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Help and Support Answers Summary

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Message 1 of 22
herzinj
9043 Views, 21 Replies

Help and Support Answers Summary

I’m trying to provide a spot to highlight (in simple form) the questions that were asked and solved in the past weeks from the Help and Support forum.  I will try to go through all of the posts from the previous week and post just the questions and answers here so that the community members can quickly scan through to see if their questions have already been resolved.  In addition, this will hopefully help encourage those who get a question answered to check it off as solved so that I can add it to this list moving forward. Thanks to all of you who have been contributing to these answers, keep up the great work!

 

James

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21 REPLIES 21
Message 2 of 22
herzinj
in reply to: herzinj

Here are the solved issues for the week ending 7/6/14.

 

Special thanks to TheCADWhisperer, andersbitsch, joseph.shi, matt.pooley, joel.palioca, jakefolwer and innovatenate for providing accepted solutions!

 

Rendering is too "zoomed out"

Q:  When I try to use the cloud rendering service, a lot of the times my models are so "zoomed out" and far away. I'm trying to zoom in real close to a certain part of a model and just render that section. In Fusion 360 I zoomed in to the angle I want, and I then I click to set that "set distance" as my home view. Sadly in the cloud rendering service it seems to use the "fit to view" look instead.

 

A:  A way to achieve this might be by using Named Views. Zoom into the region of interested on the model, then in the model browser right-click 'Named Views' and select 'New Named View'. This will save a view at the current angle & zoom level (you can edit the name of this view for easier reference later). Next time you save a version of the model, renderings of your Named Views should also appear in your cloud rendering list alongside the standard views. Does this work for you?

 

Snap to other components/sketches in sketch mode?

Q:  I can’t figure out how to snap to other components in sketch mode. For example how can i sketch a circle on a face of one component so that it is aligned to the center of a cylinder as another component/body? Another thing would be to sketch on top of another sketch while referring to the first sketch. For now i can only manage to snap to points on the sketch plane.

 

A:  When you create a sketch on existing geometry what you can do is project the existing geometry to the sketch.  This should allow you to align your circle to the center point of the cylinder.  Below you can see the options we have for projecting geometry onto a sketch.

 

 

 

For your second question, using project should allow you to project the specific areas of the other sketch onto your current sketch.

 

 

 

Lofting Help

Q:  I'm having trouble make Loft work. Is there a tutorial available to get me going.

A:  When selecting the profiles - click inside the circles, not on the circles.

If you are going in a straight line - you don't need the centerline path sketch.

 

 

 

Unkown Exception when uploading file.

Q:  Currently recieving this error - Unknown exception when uploading file. 

Also recieving this error - Unable to upload due to file being checked out. Upload will be retired.  

 Win 7 - Anyone ideas ?

 

A:  We believe these messages are being caused by a piece of data being in an invalid state on one of our servers. So we can track down the specific data causing issues, could you attach a recent log file from the computer which is seeing problems. Please send them to us.

 

Log files can be found in the folder %LOCALAPPDATA%\Autodesk\Autodesk Fusion 360\<User Specific ID>\

They are named 'AppLog<Date>.log

 

Lagging to the point of not being usable

Q:  I am using the trial on my iMac 27". I'm finding that everything is very unresposive/laggy. Even simple operations like selecting surfaces, moving selections, zooming and changing aspect are preceded by a 1-3 second lag.

 

 

A:  Take a look at your graphic effects in the models you are running.  Can you uncheck all of these options and see if that helps with the issues you are having? If not could you upload me images of your current settings for these areas?  Anti-aliasing did the trick.

 

 

 

 

Crashing when converting timeline to direct modeling

Q:  I can't get Fusion to convert the timeline to DM for the life of me. Every single time I try this command I get a crash.

 

A:  The latest update fixed this issue.  I tried this and the conversion was instantaneous. 2.0.1149

 

move function

Q:  i am new to fusion 360..i saw many tutorial and tried to learn but there is one thing i don’t get at all.  In one tutorial the person created a lamp. He used MOVE command to adjust one side but when i try to do it the whole body gets selected and whole body starts to move.   

A:  In order to use the Move Command on faces, you need to first Create a Base Feature and enter Direct Edit mode.

 

Note the difference in behavior for the move command for the following procedures:

  1. 1.      Create Fusion Design
  2. 2.      Model Ribbon > Create > Box Primitive > create a box...
  3. 3.      Select Move from Right Click Menu
  4. 4.      Try to select a face of the Box

 

Compare to Direct Edit behavior:

  1. 1.      In Fusion Design, Model Ribbon > Create > Create Base Feature command
  2. 2.      Model Ribbon > Create > Box Primitive > create a box...
  3. 3.      Select Move from Right Click Menu
  4. 4.      Try to select a face of the Box
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Message 3 of 22
mbraga0001
in reply to: herzinj

What if we use Google Sheet to assemble a matrix with this summary ?

The link below is a Sheet with this content as example.

 

https://docs.google.com/spreadsheets/d/1GMRywosLRjNpxVnXSEgAryHm8wfhCdMYmQQpeFUIVIU/edit?usp=sharing

 

I think classification (and sub-classifications) is the key and a Sheet may be a good tool for that.

Left columns (A for now) can carry on such classifications.

Message 4 of 22
herzinj
in reply to: mbraga0001

This definitly does need some additional organization, especially as the list grows.  The long term plan is to create a Community Knowledgebase, where each of these questions can be topics of their own article and community members and employees can add additional information such as video in an easily searchable fashion.  In the mean time, perhaps something like a Google Sheet or the sheet that @artygal12 is working on.  It is the same general concept as all of this, but in more of a comprehensive documentation style (https://www.sharelatex.com/project/53ac4d9081fb77e67efb58f3).  I'd love to hear your thoughts and suggestions from anyone else.

 

James

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Message 5 of 22
mbraga0001
in reply to: herzinj

I understand the idea is to capture forum content, that is a great idea despite very difficult.

The idea of a (shareable) Sheet is almost opposite the idea of Documentation or a Wiki.

The Sheet carry on small information in thousands of contents (lines) and is dynamic. Forum content are, many times, are like that.

Advantages with Sheet is:

1) Line identification (UUID): Location should be easy and direct. It make easier to reference theses lines in the forum.

2) Attributes: Allow filtering. Help identify structures. New content can be easily included in near lines.

 

Message 6 of 22
herzinj
in reply to: herzinj

Here’s the roundup of solutions for the week ending 7/13/14. 

Special thanks to those who contributed to the solutions: Al.whatmough, Joseph.shi, JDMather, TheCADWhisperer, Keqingsong, Innovatenate and Cmiller66

"The operation could not create a valid result" when shelling

Q:  When I try to shell from the flat face so it's 3 mm thick, it gives me the error "The operation could not create a valid result" and tells me to try changing the input geometry.  

 

Is this error due to the part having geometry less than 3mm thick?  Is there some workaround?  Additionally, what's with the tangency check box option?  Is that something that can make a difference in this case?

 

A:  The shell command generally is used to convert solid body geometry into a thin walled solid body. It sort of excavates the internal volume of a solid and converts it into a vessel. Any faces selected in the shell command should be remove. An easy example is to start with a solid cube. The shell command can quickly turn the solid cube into an open "crate" or "box."

  

Where the shell command can get tricky is with organic, "curvy" shapes. The command doesn't do well when the results "overlap" onto itself. This tends to occur when the Thickness value is too large in the shell command or the Body is too thin. You may find that you can get the shell command to work by reducing the value from 3 mm to 1 mm. You should be to find the thickness at which the shell command fails. You may be able to change the Direction of the Shell from Inside to Outside to work around the issue.

 

 Looking for something like project sub folders

Q:  I am wondering if there is more organizational capability than I have figured out.

 

A:  You can create folders inside one project as you like from "Data" tab:

1.Click Data tab

 

 2.Click any of the projects and you will find the "New Folder" icon on the upper right corner

 

 3.Create any folder you like and you can move the design from any folder/ subfolder to others.

 

extrude problem (there's got to be an answer to this)

Q:  To create a bolt or nut this is my procedure.  I start in model, sketch the profile for 1/2 the head of the bolt.  Do a revolve.  On the face of what will be the bottom side of the bolt, sketch a circle the same diameter as the head (distance across the points) and then draw a line from the center to the circle.  Array the line by 6.  Draw 6 lines from outer point to point, then extrude a cut in this area to create the flats of the bolt head.  Then simply extrude a circle from the center of the lower face the length required.  This method worked just fine before the latest version of the program was introduced.  Now the extrude cut I try to do refuses to only cut the sections I ask for. It extrudes the entire head.

 

 I've tried to attach this file but all I get is "The contents of the attachment doesn't match it's file type"  If someone could tell me what is the deal with this too.    

 

A: I simply used the Polygon tool. I am using Windows OS. In Windows OS right click on the file name and select Send to Compressed (zipped) Folder to attach file here.

 

Boundary Fill problem

Q:  I am trying to remove the geometry between the two surface bodies.

I think I have done this in the past on this same part (modeled in different way) but now I cannot get it to work. As soon as I try to Select Cells the solid and the surface bodies vanish.

  

A:  For the first selection I had only selected the "cutting surface bodies", I hadn't selected the solid body as well.

  

Confused about components

Q:  I create a lot of small, simple parts (bolts, nuts, stamped metal, cut from plate, cut from tube, etc.) and then bring them into an assembly.  I do this because many parts are reused in other assemblys.  Sort of a pull parts off the shelf and assemble method.  What I'm wondering about is should my single parts be converted to components when they are created or should they be turned into components after I insert them into an assembly?   

 

A:  Your single parts should be converted into components prior to assembling them with joints. The main different between bodies and components is that when bodies are converted into components, the components each have their own origin planes. Also, when converting a body to a component, that original body gets stored in the new component's sub-structure. 

Move sketch from one component to another

Q:  Is there any way to move a sketch from the general sketches folder to a sketch folder within a sub component?  For example, I make a new sketch and then extrude the sketch into a new body. I then convert the body to a component. I want the initial sketch to be foldered in the browser under the new component, but it doesn't seem like it can move.

  

A:  One suggestion you may find is that you can copy and paste geometry from one active sketch into another. The steps to do this are:

 

1. Edit the sketch that contains the geometry you wish to move

2. Select all Sketch figures 

3. Select Copy from the right click menu or use the keyboard shortcut for Copy command (Windows CTRL+C- Mac Command + C)

4. Stop Sketch

5. Activate the Component you wish to place the sketch in (select white circle next to the Component name in the browser to Activate Component)

6. Select the Work Plane or Face you wish to sketch on, Right mouse click and select Create Sketch

7. Select Paste from the right click menu or use the keyboard shortcut for Copy command (Windows CTRL+V- Mac Command + V) while in an active sketch.

8. Move Geometry as necessary (if necessary)

9. Stop Sketch

 

Note: New sketch will be created with identical sketch geometry. You may need to activate the top-level of the design to get back.

 

2D Drawing Units

Q:  I created a part using metric units. When I create the 2D drawing the units are in inches. How can I change the units? 

 

A:  For drawing units and other default drawing settings, please expand the main (3-bar icon) menu > Preferences > Drawing.  These settings will be applied for all new drawings you create.

 

A sub-set of these settings are also available for the existing drawing you have open .  To change these see Document Settings on the main menu.  Here you can change sheet size, text height, dimension precision, etc.but changing Units for an existing drawing is not currently supported.

  

Sketch - constrain by formula

Q:  Can I define the value of a dimension by a formula ?

 

 A:  Notice that I made one dimension a function of another simply by typing in the equation.

 

 If you want to - you can rename the dimension variable names. Here I named them Arm and Leg.  Fusion replace the autoassigned d1 and d2 with the new variable names in the equation.

 

 If you create your User Parameter variable names in advanced --  you can simply type them in as you go

  

CAM 2D programming trouble

Q:  I am trying to figure out how to set a pocket or contour using the profile edge at the top and get it to cut down from there but I cannot figure out how to do this. Normally I would just use the profile at the bottom but in some cases a other modeling operations will have changed or eliminated sections of the profile at the bottom leaving only an unaltered profile at the top or mid way up the pocket.

Is it possible to do this?

 

A:  Select the chain at the top, then use the hights tab to change the bottom of the pocket from "From Chain" to "Selection"

 

You can now select a face you want to operation to go down too.

 

https://damassets.autodesk.net/content/dam/autodesk/logos/autodesk-logo-primary-rgb-black-small_forum.png
Message 7 of 22
herzinj
in reply to: herzinj

Here is the roundup for the week ending 7/20.  Special thanks to Innovatenate, Fonsecr, Schneik, SallyYang, Wendy.Chen_Autodesk and TheCADWhisperer for the solutions they provided.  Keep it up!

 

Loft Functionality

Q:  Is it possible to create a Loft between these two arc sketches in Fusion 360?

 

A:  Have you tried using the Patch workspace > Create drop down menu > Loft command?

  

You may also consider Using the Extrude command in by using the Create Form or working within the Scuplt workspace. See the video below for detail.

https://screencast.autodesk.com/Main/Details/977ebbff-3c38-4069-8915-64f2a1890b68

 

 Vase with polygonal appearance!

Q:  Do it with the t-spline using the tool face in "Display box" seems simple. But the result is not what you want, then it is not exportable.

 

Adding the edge ... it becomes complex to control!

 

A:  You may be able to use a quadball to create a similar shape. See the video below for further detail.

 

 https://screencast.autodesk.com/Main/Details/56c37604-302b-4679-874c-5a983822e6ce?t=8.588s

 

Problem in applying material to an extruded object

 

Q: I was doing the tutorial (razor) exactly, but my body is not changing when clicking the material part.  I've tried new project and just basic ball wasn't changing either. I choose the bodies first and clicked matrials option, but after clicking it, the selected body turns into blue line which I think it should be whole blue body.

 

A:  Yes, currently after clicking the material, the highlight will become the blue line.

http://forums.autodesk.com/t5/Design-Differently/Making-it-Look-Good-Apply-and-Edit-materials-in-Fus...

 

t-spline body conversion error

 

Q:  When I tried to get out from sculpt mode, there is t-spline error.  I know what this error means, but don't know how to solve it. If I could know which specific part is causing the error, I can adjust it again, but I don't know which part it is. Is there any way that I can figure out which part is causing this error?

 

A:  Go to Modify>Utilities>Repair Body while editing the Form and select the body and look for red Star Points.

 

How do I copy just a sketch from one desing to another?

 

Q:  I created a sketch in one design that I want to copy to another. 

 

A:  1. Edit the sketch that contains the Sketch geometry you wish to copy (you should see the Stop Sketch command appear on the right side of the ribbon if you have edited a sketch)

2. Select all Sketch figures by dragging a selection box around them (the sketch figures will highlight)

3. Select Copy from the right click menu or use the keyboard shortcut for Copy command (Windows CTRL+C- Mac Command + C)

4. Enter into the Other Design's workspace by clicking on the tab above the upper Toolbar

5. Activate the Component you wish to place the sketch in, if necessary. (Hint: select white button next to the Component name in the browser to Activate Component)

6. Next, select Model > Create > Create Base Feature (Finish Base Feature will appear on the right side of the Ribbon)

7. Select the Work Plane or Face you wish to sketch on, Right mouse click and select Create Sketch (the Stop Sketch command appear on the right side of the ribbon)

8. Select Paste from the right click menu or use the keyboard shortcut for Copy command (Windows CTRL+V- Mac Command + V) while in the active sketch.

9. Use the Move command to position the sketch

10. Select OK in the Move command to place the sketch

 

See the ScreenCast below for a demonstration.

 

https://screencast.autodesk.com/Main/Details/a9bc9f69-a583-4b9a-a50a-268d6f1c710b?t=3.228821s&autopl...

 

Performance Issues after Converting BRep Faces

 

Q:  I have had no significant performance issues until I converted some Brep faces. No matter what I do it freezes up when I scroll around in the interface. It is really bad when I zoom in and out.

 

A:  The Convert command is defaulting the Deviation values to 0.000in, which shouldn't be the case. T-Splines conversion will calculate a match of the input surface within these 'Deviation' tolerances, so with tolerances as low as this, it's trying super-hard to match the input surface precisely. This results in a lot of computing (= slow performance) and in the end will result in a T-Splines body with a lot faces (= large file size, and not a very practical T-Splines model at the end of it).

 

 I'd recommend raising these Deviation values (both of them) to an acceptable tolerance first, then click the model in the canvas. Or, in the Length Spacing menus, choose Uniform, which allows you to specify how many T-Splines faces you have in both directions.

 

 If you've already converted other parts of the model to T-Splines, I'd recommend re-converting those following the process above as well, which should cut down on the file size.

 

Dashboard shows only black screen

Q:  I have updated to the new version of Fusion 360 (supporting CAM) and when I now try to log into Fusion I get a black dashboard screen.  Drop down menu works – was able to start recent design and enter drawing mode, but dashboard still black.

 

A:

  •         Run command  "dxdiag"  to launch "DirectX Diagnostic Tool" dialog and switch to "Display"
  •         Capture the "Device" and "Driver" part and send to us
  •         Upgrade the graphic card driver to the latest 
  •         Try dashboard again and let us know the result

 

Unable to edit face

Q:  I am trying to recreate a shoe last from a 3D scan.

 

I have built the general shape by slicing the scan and tracing the outline of core parts of the last. Then i have used the loft command to connect every sketch.

 

Now i want to make the last adjustments to the shape to make it fit the scan more precisely. This i want to do with the Edit face command.

 

But every time i try to pull or push a face, even in the smallest manner, i get an error messages saying that it is not able to replace the face.

 

It sometimes changes whether it calls it "Camfer/fillet" or that it is unable to replace the face. 

 

A:  The error message appears to be an issue with the rebuilding the fillet command once the edit face command is completed. I note that if delete the fillet command, the Edit Face command will execute successfully. 

 

A couple of suggestions you may try is to use the Sculpt > Loft command first. This will generate a Sculpt Body (T-Spline body) which can be convert to B-Rep geometry later after the clean up is done.

  

Another trick may be to use the Patch > Loft command to create a surface body initially. This is much easier to manipulate in the Edit Face command since the geometry doesn not have to convert back to a solid body, but can simply become a surface body (no enclosed volume). After you are done tweaking with Edit Face, you can use the Sculpt > Patch command to close up any open gaps in the surface. Next, use the Sculpt > Modify > Stitch command to convert the surface bodies into a solid body. See the below video for detail.

 

https://screencast.autodesk.com/Main/Details/2ceb2c22-3591-4236-934c-4e0f815eb2a8

 

Change view to construction plane

Q:  When I create a construction plane through an edge of a solid, the edge does not seem to be part of the plane. I cannot lock to it or use the edge to constrain other elements in the plane.    

A:  While in Sketch are you using the Project Geometry tool?

 

How can I join these using a path that isn't straight?

 

Q:  I have to pieces that I can extrude the faces on, but I'm not sure how to join them using a non-straight form.

 

A:  Start the Loft command and select the rectangular end faces.

Click on Profile1 and set it to Tangent.

Click on Profile2 and set it to Tangent.

  

Here is another technique using Sweep

 

Sketch your path.  (this is just an example - the path can be whatever you want it to be)

 

and then sweep a profile.

  

Model corruption after assembling components

Q:  I feel like Fusion 360 created some internal corruption during the assembly process to where it thinks there is a bogus body, component, or feature out somewhere in infinity.  This time Fusion has zoomed out my model to make it unworkable. 

  

A:  Take a look at KneeFlxExtPstAssy.  If you turn this parts origin on you will see it is WAYYYYYY off in space.  Deleting this part returns the design to a normal view extents. 

STEP File to Inventor LT Feature recognition

Q:  I have opened a STEP file in fusion 360 and used the find feature process and saved the file as a new version Fusion 360 finds the features OK.  When I open the file in inventor LT 2014 the features recognized by Fusion 360 are not displayed all I get is the dumb solid again.

 

A:  When fusion finds features these are direct features, not features with history. These features will not come over to Inventor LT.  I would get the Inventor feature recognition app from the exchange app store.

 

Finishing (CAM)

 

Q:  Is  there a way on Fusion 360 to machine a 3D contour just of a face, in this case just want to machine the interior curved face on other direction I can do that with parallel, put it select all the surfaces nor just the one curved side.

A:  Set the machining boundary for the Contour operation to machine with the "tool center" going to the Silhouette. This is controlled on the Geometry tab (the 2nd one).

 

 

 

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Message 8 of 22
herzinj
in reply to: herzinj

Here is the roundup of solutions for the week ending 7/27/14.  Special thanks to innovatenate and TheCADWhisperer for their help on these topics.  

 

Can I undo a thicken from a previous version?

 

Q:  I opened up a file that I was working on last night and this morning I wanted to add some more faces in the sculpt environment which I could thicken to be a part of the old body. I'm trying to find a way to undo the thicken from last night, but I haven't found anything. I'm also trying to load an old version, but Fusion seems to be crashing on me when I do that. Is this a possible feature in Fusion?

 

A:  When working in the Create Form command, you are in a Direct Edit mode. This means that you will either have to "unthicken" the sculpt body manually. 

 

When trying to open an old version. Close the design and open the item details from the dashboard (select the name of the design to bring up item details). In the Versions panel, use the Promote command (see below image) to make an old version the current version.

 

 Last, use the Edit command to edit the freshly promoted version. Note that you should see the version number increment after using the promote command.

  

Is it possible to edit a Sculpt object in the Model workspace?

 

Q:  I was working on an object in the Sculpt workspace and I wanted to edit it in the model workspace, but I'm not able to sketch onto any of the faces of the Sculpt object no matter what workspace I'm in. More specifically I want to extrude cut shapes through the body below which was made using thickened faces.

  

A:  You cannot sketch on a face sculpt body. You also cannot edit a sculpt body from the Model work space. Whenever you finish form, the sculpt body automatically gets converted into a solid (B-Rep) geometry. This can be very powerful when combined with the Timeline since the model features will update when you make edits the sculpt body.

 

A couple of suggestions for a solution are below.

 

In the model environment, you can sketch on a planar (totally flat) face. One thing you may consider doing if you do not have a planar face to sketch, is to create a work plane in the position that you need to sketch on. Then use the extrude (cut) feature to remove material from the solid.

 

Another option is to create sketch on the default plane in the shape that you need a cut out in. Next, convert this sketch into a solid body by extruding the sketch into a solid body. Now, use the move command to position the body where the cut should be. Don't forget to use the reorient command in Move to help position the solid body. Once positioned, you may use the Model > Modify > Combine command to do a Boolean Cut and remove material.

 

You may also convert the "cut shape" body to a component and then use assemble > joints to position the component. After position, you may again use the Combine command to subtract one component from another.

 

Another option is to use the Project to Surface command to project a sketch onto a complex surface in the Model work space. Next, create a Patch in the patch work space and thicken the patch to remove material.

 

I've made a ScreenCast of these suggestions (below). Take a look and let me know if helps.

 

https://screencast.autodesk.com/Main/Details/0caa5b12-b911-4d54-b78b-c45cda8d8542

https://damassets.autodesk.net/content/dam/autodesk/logos/autodesk-logo-primary-rgb-black-small_forum.png
Message 9 of 22
herzinj
in reply to: herzinj

Here is the solution round up from the week ending 8/3.  Special thanks to rpagewood, innovatenate, TheCADWhisperer and matt.pooley for their accepted solutions this week.

 

Can't create new design or upload CAD data or Open Designs 

 

Q:  I'm running Windows 8.1. I'm running version 2.0.1193 of Fusion 360.

 

I can't:

  •         Open designs - click and does nothing at all
  •         Upload CAD data - opens an empty modal window 
  •         or Create Designs - opens an empty modal window 

 

A:  I just wanted to add a note that performing a clean uninstall and re-install resolved the issue. 

 

What's the easiest way to create the shaft in this sketch?

 

Q:  There's an interesting article about sketches at http://forums.autodesk.com/t5/Design-Differently/The-Power-of-Top-Down-Design-in-Fusion-360/bc-p/517...

 

But there's some features of the sketch that are non-obvious.

 

1.  If you've got the two circles for the pins on the shaft, how do you create the shaft itself?  Is there a simple way to do it, or is a muti-step process involving intermediate circles that get deleted?

 

2.  What's the dotted line in the circle?  The inner and outer circle seem obvious (they're just circles), but that dotted thing seems to be some sort of joint or constraint.

 

3.  How do you get a dimension that's just the distance between the two pins?  It seems like creating dimensions always wants to draw at 90 degree angles, never just the distance between two points.

 

A:  I can walk you through this design step-by-step.

 

Start a new design.

 

1. Change the Units to inch

2. Start a new sketch on the XY plane and then select the Project Geometry tool and project the Origin.

3. Sketch a circle centered at the origin.  Dimension the circle 1".  Right click on the circle and select Construction.

 

1.png

 

Sketch 2 more circles at the origin as shown.

(You can see that the dotted linetype circle is construction linetype.)

 

2.png

 

Add the rectangle and dimension as shown.

 3.png

Add this construction line (you know how to create a construction line now, this step is not shown in the original sketch).

 4.png

Sketch small circle at intersection of the construction line and construction circle.

Sketch small circle to left as in image.

Sketch construction line between the two small circles.

Dimension the length of the 3" construction line by Right Mouse Button - Aligned.

Add an Equal (=) constraint between the two small circles that we you just created.

5.png 

 

Sketch 2 larger circles at the centerpoints of the 2 smaller circles.

Sketch lines connecting them together (Tip: If you click and drag - Fusion will automatically add the Tagent Constraints.  If you don't get the automatic Tangents, add them yourself).

 6.png

Trim the two arcs.

Add an = constraint between the two arcs.

Dimension one of the arcs.

Stop Sketch

7.png

Export Archive.

Right click on the exported archive file and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here (or the *.f3d if the forum will allow).

 

Unkown Exception when uploading file.

Q:  Currently recieving this error - Unknown exception when uploading file.

Also recieving this error - Unable to upload due to file being checked out. Upload will be retired.

Win 7 - Anyone ideas ?

 

A:  We believe these messages are being caused by a piece of data being in an invalid state on one of our servers.

So we can track down the specific data causing issues, could you attach a recent log file from the computer which is seeing problems.

 

Log files can be found in the folder %LOCALAPPDATA%\Autodesk\Autodesk Fusion 360\<User Specific ID>\

They are named 'AppLog<Date>.log

 

Please attach log files from the last 48 hours, that should include enough information to track this issue down.

 

Is there a way to measure volume (or mass if given density) of a body?

 

Q:  I would like to measure the volume of a body in order to figure out what its mass would be. Is that easily possible in Fusion 360?

 

A:  You can get those properties by right clicking on the root component at the browser and select properties: Two screen shots to show you here:

 

 

 

Helical sweep

Q:  I have been trying to create a reel for a reel mower. The reel blade is essentially several metal bars with a sharpened edge that have been bent along a helical path and then welded to a number of circular metal plates. I tried to create this in Fusion 360 but gave up after a few hours. I was using the coil tool with a small (0.1mm) triangle section and then sweeping my profile along this shape. 

 

The problem I'm having is that the profile seems to be pivoting around the point where it touches the path, as well as rotating to keep up with the helix. This means that by the time it has reached the bottom of my path, the cutting edge points in to the middle.

 

A:  There is an option in the preferences to enable 3D sketching of lines and splines.

 

8.png

 

I use the Include 3D geometry feature to generate 3D splines to act as guide rails for the loft. The below screencast is from another forum thread, but it may help here too.

 

Sketch Geometry Overconstrained

Q:  There doesn't seem to be any logic behind it and the message doesn't offer any indication of which constraints are causing the problem.

A:  So it turns out that I had some of the sketch geometry fixed as well as being driven by constrains and dimensions. It would be nice if the pop up messages offered explanations rather than just giving a warning. I shouldn't need to come and post here every time I can't figure something out.

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Message 10 of 22
herzinj
in reply to: herzinj

Here is a summary of the solutions for the week ending 8/17/14.  Hope these help and please let me know what questions you still have.

 

T Spline Join

Q:  I have a three-fold question regarding T Splines.

 

I would like to Intersect / Join / Merge 2 T Splines.  

 

Second, I would like to create an edge that follows a curve.  

 

Lastly, can I slice a T Spline?  

 

A:  You could think of T-Spline bodies as networks of faces and each face is tied to another face at an edge.  This means when modeling the T-Spline body you are always working to build that network so it represents the shape you are looking for.  It is possible to create sharp transitions between faces with creases.

 

In the example you are showing you could convert the T-Splines into BRep solids and use the Combine command in the Model - Modify menu.  At that point you will have a sharp transition between the two T-Spline bodies.  That is one strategy.  If you are using a parametric/timeline document you could go back and edit the Form node to refine the shape and upon selecting Finish Form the combine operation will update.  This is how you would handle Slicing the T-Spline as well.  Convert it (which happens automatically in the parametric document) and then use a curve or plane to Split Body.

 

You could also develop the T-Spline body to develop the shape you want.  You can start with a simple primitive and through inserting edges and extruding faces create a more refined shape.  I am attaching an example file with some T-Spline bodies that may give you some ideas about how to develop the form.  Check out the learning materials under the Form area to get more information about developing the T-Spline form.

 

 

Fusion 360 install problem

Q:  I have tried installing Fusion 360 on my Windows 7 Home Premium machine. After getting through about 75% of the process the installation fails with the error "......\acdbradres.dll has already been installed and cannot be delivered twice".

A:  The problem may be that the "web deploy" folder is in a state where the installer thinks it's being written to. 

 

**Thanks for your suggestions, it solved the problem.**

 The directory I found was "Web Deploy", which I deleted.

 The installation went fine afterwards.

 

Other Suggestions:

1. Re-starting your system and login.

2. Launch My Computer and go to c:\users\<yourusername>\appdata\local\autodesk.

3. Check for the following folders and if present, delete them:

  •         Autodesk Fusion 360
  •         Web Services
  •         Web Deploy
  •         Neutron Platform

4. Next close My Computer and try re-installing.

 

 

 

 

Would somebody mind telling me what that "stop" or danger sign is near the body

Q:  What is the “stop” or danger sign near the body

 

A:  That looks like the icon for selectable/unselectable. This option is available from the right click menu of a body or item in the Browser.

 

The purpose of selectable/unselectable toggle is to allow the visible display of a body or component for visual reference without it interfering with selection.

 

Fusion 360 crashes

Q: Every time, when I try to launch Fusion 360 it crashes every time.. I tried to install new graphic cards drivers and delete Inventor prifle but it didn't help.

Nothing happen when I launch Fusion 360. I got only Fusion 360 report error.

 

A: It looks like this should be resolved with R1 that is releasing tomorrow.

We found that the issue was with having Western European characters in your user name.

 

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Message 11 of 22
herzinj
in reply to: herzinj

Here is the solution roundup for the week ending 8/24/14.  Thanks (as always) to TheCADWhisperer and Innovatenate for their answers!

 

Press Pull / Extrude from T-Spline at right angle

Q:  I have created a T-Spline shape, and then enlarged one of the sides.  I want to then Extrude (or Press/Pull) that side directly out.  The problem is, is that one I finish the T-Spline form, I can select one flat face, but the Press/Pull command extrudes out the face in the same direction as the T-Spline shape originally indicated.

 

I desire that shape to be extruded directly on a 90 degree angle.

 

A picture is worth a thousand words...I want the blue area to NOT continue up the slope, but to extrude out directly sideways to make a sharp angle, NOT a continuation of the slope.  In my example, I have finished with the form and am using the Model-->Press/Pull command.  

 

1.png

 

A:  Turn on the visibility of the Origin Workplanes

Offset the appropriate workplane (I didn't know what distance you might need).

Create a new Sketch on the new Workplane.

Project Geometry the face you highlighted.

Loft from the Sketch to the Face.

 

Fusion 360 extremely long to startup and only works in offline mode

Q:  I'm using Autodesk Fusion 360 v2.0.1193, and since tonight, Fusion takes around 5-8 minutes to start up. When it eventually does, it only runs in offline mode?

 

I've tried restarting the application, restarted my Mac? Any ideas what could be wrong?

 

A:  While in offline mode, you may use the export archive command to create a *F3D file that is stored on your local hard drive:

1. Open Fusion 360 (Offline Mode is okay)

2. Open the design

3. In the main menu, select Export Archive

4. Save the *.F3D file on your local hard drive.

5. Back-up the archive file to a safe location

 

For the connectivity issue, is there anything different on your network that would prevent Fusion 360 from accessing the web (e.g. a new router, updated security software/anti-virus)? Are you currently able to access the internet on that machine?

 

 

Extrude projected sketch

Q:  I created a 2D sketch and projected this on a surface of a converted sculpted body. I can clearly see all the nice red lines but have no possibility to select them when extruding. I would like to cut that sketch about 1 mm deep from the top of the surface.

  

2.png

 

A:  Can you Split the face and Thicken-Cut?

 

Another option (depending on design intent) would be to offset the face as a surface and then Extrude cut to the offset surface.

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Message 12 of 22
herzinj
in reply to: herzinj

There were a lot of great solutions provided this week.  Thanks to everyone who helped get these answered: Kingson138, SallyYang, andrewsears, rishivadher, Innovatenate, Ron Russell, Bud.schroeder.

 

History - group/ungroup history, rearranging grouped history

 

Q:  In the history timeline, after you group some functions together, a "+/-" symbol appears. I see that you can expand/collaspe the group, but how do you ungroup them?

 

Is it possible to drag history functions in/ out of a history group?

 

A:  We currently don't support drag & drop items into a group. However you can delete the group and then reform it with new items. To delete a group, you can collapse the group and right click on it to invoke delete function, then select "Delete group and expand its contents ".

 1.png

 

subdivide on manifold surface

Q:  On some surfaces I can apply subdivide (for T-spline manipulation) and on some I get the error: subdivide operationon can be applied only on manifold surfaces.  What is a manifold surface?

 

A:  When we say the part needs to be a manifold part, it means that somewhere on your model you have 1 edge touching more than 2 surfaces.

 

Here is an example: This part comes to a point an edge at the blue highlight.  1 edge touches 4 surfaces.  This is a non-manifold part.

 

2.png 

 

Importing DXF & selecting units??

My question is when I upload a .dxf is there a way to select scale? IE how I let fusion know if its importing in inches/mm etc... If there is no way of selecting this what is Fusions default scale for DXF imports?

 

Go to preference and chose the mm to be your default unit our same as the DXF, which you’re importing.

Are driven dimensions available and how do I delete a sketch constraint?

Question 1: Are driven dimensions available in Fusion 360?

 

Question 2: How do I delete a sketch constraint?

 

A: With respect to driven dimensions:

 

Reference and driven dimensions are not available at this time. However, you can drive dimensions through expressions in the parameters dialog with timeline is enabled, which may help. To access this dialog, select the "Change Parameters" command in the Modify panel of the Model workspace. 

 

There are some IdeaStation post in about this if you would like to vote:

 

http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/driving-dimensions/idi-p/5039950

 

http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/visible-dimensions-in-3d-space/idi-p/...

 

With respect to deleting sketch constraints:

 

To delete a sketch constraint:

Step 1: select the sketch constraint (must be editing the sketch)

Step 2: press the delete key on the keyboard or right click and select delete while the sketch constraint is selected

 

I should note that you can use the “select other” tool (just linger on  the left click button to access) to select tricky sketch geometry constraints. This may be helpful if you dealing with a really crowded sketch.

 

Rotating an SVG file?

Q:  How do you rotate an SVG file?

A:  If you are in Direct Edit Mode, you can use the move command to rotate a sketch. You may try right clicking on the sketch in the timeline and selecting Convert to DM feature. Now, edit the resulting Base Feature in the Timeline and you may right click on the sketch in the Browser and choose move. The move triad will have an options to rotate the sketch.

 

Please note that if you have any fixed sketch entities, this may impact the behavior of a move command

  

I've a made a ScreenCast that shows how I might tackle this issue, below. 

 

 https://screencast.autodesk.com/Main/Details/5ef66622-5318-4c10-93e6-1b8e68dea84d?t=3.10072s

 

Beginner problems: How to use the pull command for locally fitting spline?

 

Q:  My questions tend to involve scenarios that are hard to explain, so there a five screen captures along with my text. But they didn’t paste into the composition window of the forum, so you’ll just find the text below. The text with pics are in the attached pdf file

 

Hi, I’m deeply intrigued by Fusion 360, but I’m stumbling a bit the sculpt workspace. Could you help me with my baby steps?

I’m working on a head for fun. It currently looks like a platypus (how that happened is another post J) but here I’m focused on creating an eyeball. In particular, I’d like to use a solid model, such as a sphere, to trim the grid I’ve already put in place (FIG 1):

With timeline magic, I put the construction of the sphere, the fitter or trim object, before the sculpting of the spline. So the first three actions below, the creation and the two moves, were done originally with the face in place, after the spline creation, so that I could align the sphere (FIG 2):

 

Problem 1: disappearing and unselectable body element in browser, but forced display

You’d notice that I put in a component creation action in the timeline just before I create the spline. That’s because the sphere object otherwise is unselectable.  I would have expected that I could select it as shown (FIG 3)

The sphere doesn’t even show it the browser.But it is displayed and in fact prevents me from selecting the faces of the eye socket (unless I left-click-and-hold, which now explicitly also reveals that the sphere object is in fact still there). This disappearance act is somewhat baffling but once I componentize the sphere, then I won’t hide in sculpt mode.

Did I baby step my way into a bug or a feature here?

 

Problem 2: the pull command doesn’t behave

With the sphere in place, I’d like to pull the vertices of few faces in the eye socket to the sphere, so I prepare the pull commands as follows (FIG4):

The auto select option of the command uses I-don’t-know-which target to create a wacko cubist painting of sorts. So I select the sphere explicitly (that’s why componentization is necessary!). Then my head turns into this medussa (FIG5):

And that’s for trying to align the 9 spline vertices to the sphere. Can you explain what happens?

 

Problem 3 How do I make a simple trim according to the sphere?

Related: can I simply cut out the intersection of the sphere with the selected surfaces of the spline? I’m not after an exact projection of the fitter object onto the surface, just something that’ll locally tessellate the involved spline surfaces so as to approximate the surface curve (which may itself not be spline representable).

 

A:  Problem 1: disappearing and unselectable body element in browser, but forced display

Well, I still don't know whether this is a bug or feature, but Paul explains the solution in the video.

 

Problem 2: the pull command doesn’t behave

I followed the observations above (valid or not!). In particular, I had to cleave the sphere to get surface pull to work; with only the front half in place I was able to use the pull command after having meticously worked the grid with control point snapping. Control point snapping itself behaved better with the full sphere.

 

Ron suggested that "You appear to have selected entire faces rather than vertices, that could give startling results with the Pull tool." but initially selecting faces (with vertices and edges) was not the issue: the command only retains the 9 vertices.

 

Problem 3 How do I make a simple trim according to the sphere?

 

The result of the properly prepared pull command gave the spline shown below. Now clearly there's a set of faces whose boundary approximate the intersection of the sphere. But there is no "simple trim" -- this is big mouthful.

 

3.jpg

 

Project Privacy Settings not working?

 

Q:  How do you start a private project, that is not viewable to any one?

 

When I started a project, these are the "Content and Privacy Settings":

 

  •         Project type: secret"
  •         guest access: "disabled"

 

Even though I have these settings selected, when I check my project file, it seems like it is still being viewed by someone (please refer to the attached photo).

 

Or does the "eye" icon in the photo mean something else?

 

A:  I was able to take a look at this in Fusion and the views get marked each time you view or refresh the page. I see this behavior in both Fusion and Autodesk 360, so I went ahead and reported this to the QA Team. I also verified that no one can see a project unless you invite them into the project. 

Inset edge in parametric mode...how to offset by specific distance

 

Q:  I have a cylinder I created in Sculpt mode with some nice curves to it.  The thing  I am trying to reproduce has a small bump that starts out at 2.5mm below the top.  

 

When I "Insert Edge" I only get a number between 0 and 100 percent, and not any specific distance.  Maybe parametric mode does not support this, but I want to say "Inset edge 2.5mm away from the edge I selected to start the insertion from".  This functionality should not be constricted by the "next" T-sline line...If I need something 2.5mm down the object then that is where I would like to put it.

 

I realize that the Sketch environment allows for precise measurements, but I want to create a beautiful T-sline curve...I just want to start and end it at the right place.

 

I also tried creating construction planes but ran into a couple of problems:

 

-construction planes cannot be offset/selected from a T-spline "face"...I can only select the global plane and figure out the measurements myself

-I cannot snap the "insert edge" command to a plane so I have to eyeball it

-The "Insert Edge --> Offset" functionality does not seem to do anything, even though I can select a construction plane

-The "Insert Edge --> Offset --> Measure" never seems to change...that seems liek what I am looking for but maybe offset is not what I am looking for.

 

Any suggestions on workflow, or am I going abou this incorrectly?  In the attached screenshot you can see the top of my object, and some planes I have created but again, I have to eyeball it.

 

But then again, again, Parametric Mode might ALL be about eyeballing it, and precise measurements maybe should not be expected there, especially on the side of a T-spline curve (would be great to be able to "freeze" a point on a Tspline.)

 

4.png

 

A:  Hi to offset a construction plane up and down or to any position is not possible at the Parametric Mode in this version. You have to stop recording to go to Direct Modeling Mode. Then you can go to Sculpt workspace and the construction planes can be moved to any position you wanted. I am not sure if the new update coming on September 2, 2014 will add that capability. I had been requesting that many times and nothing seems to had been done. This is in fact a missing feature.

 

If you are at the "Create Form" workspace at the parametric mode you have to "Finish form" before going into Direct Modeling Mode.

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Message 13 of 22
herzinj
in reply to: herzinj

Here is the solution roundup for the week ending 9/7/14.  Special thanks to Thecadwhisperer, Sanguish, Deyop, rishivadher, Kumara, Joseph.shi, innovatenate, and Yqliu.  This was an extremely active week on the help forums, and you all play a huge part in making Fusion 360 a success!

 

Holes evenly spaced on a circle, but under an angle to the surface

Q:  Well, my first issue: I would like to create a few evenly spaced holes on a circle. The catch: these holes must be under a 15-degree angle with the surface, thus 'pointing to the center of the circle'.

 

How does one do this in Fusion360? I tried creating a plane under a 15-degree angle, a point on the surface, and an axis through the point and perpendicular to the plane, but so far I have not succeeded.

 

A:  I didn't see your *.f3d file - so I had to start from scratch using the SWx example.

It looked to me like maybe the SWx user did too much work - so I simplified the process a bit.  (see attached *.f3d file)  (it also could have been done the same way as in SWx, but I try to avoid work)

 

 1.png

 

2.png

 

This is pretty much how I would set it up on my milling machine.  You used flat bottom holes rather than 118° drill points - so that is what I used.

 

Splitting a section of a body

 

Q:  I have an irregularly shaped section of a body that I need to split so that I have two pieces: one long piece, and the second which is shown by the face on the back of the item.

 

  3.png

 

4.png

 

A:  I stepped back through my model to before the path was drawn that was used with the sweep that created the half-circle tunnel.

 

I then make sure that the path for the 'tunnel' was in a sketch of its own.

 

Then I was able to repeat the sweep process. 

 

And then when I wanted to separate that two pieces I was able to select the body, and then then carefully select the path that was used for the sweep as the cutting tool, and it worked fine.

 

Some Entities are Degenerated

Q:  I'm trying to convert a TSpline and I'm getting an error that "some entities are degenerated".  What does that mean?

 

A:  Are you getting any visual feedback on the screen when it fails?  There should be some red highlighting where the problem occurs.  It could mean that there are multiple vertex in the same position which are not merged together.  If you can provide the example I will try to give you a better explanation.  We have updated error messages in the latest release but this error may not have been addressed.

 

Parts suspended in air - how do I drop them back down onto my original "plane"?

 

Q:  I'm not even sure how I did this...  I was simply working along and added a new cylinder and then noticed a bunch of shadows far below my parts I've been working on...

 

They're all on the same plane (except the cylinder I just added) so I obviously did this @ one time. &nbsp; How do I move them all back down?

 

A:  try to redefine the sketch plane to plane of origin. For whatever reason the 4th part I created was much lower (on the Z axis)
than the remaining parts. As I was preparing to try to move all the other
parts back to the original plane I first tried deleting this "part #4" and
doing so automatically shifted the plane up to meet the original 3 parts.
Problem solved. I still don't know how/why "part #4" was created several
hundred millimeters below the other 3 parts but the problem is now gone.

Insert Option

 

Q:  I notice that "Insert" is no longer located at the bottom of the joints pull down.  I've searched but am unable to find it anywhere.  Have I missed something?

 

A:  On windows you can now drag and drop the design from your side panel or RMB on the design and insert. On a mac we support on the RMB Insert for this release. Hope this helps.

 

OPEN not always available.

 

Q:  Most times when I launch F360, the OPEN option is not available.  It will take 5-10 minutes before I can open a design.  RARELY, is it available right after it loads.

 

A:  You now have various ways to open the design in Sep release : either right click and select "open" option, or simply double click on the design.
And now you can even open the design from web page by clicking the "Open in Fusion 360" button.

Mirror circular for only part of model

 

Q:  I am trying to model a bottle.  The bottle is slightly flattened in one dimension when compared to the other...here is a top view:

 

5.png

 

...so, no big deal to model this, as I can mirror in the X direction at the same time as mirroring in the Y direction to get this symmetric shape.  The problem is when I go to model the "cap" of the bottle.  Here is a screenshot of the canvas showing what I need to do:

 

6.png 

 

...you can see that I have modeled the bottle all the way up to the cap, but now I need to make the cap completely circular and symmetrical in ALL directions.  

 

Problem:  If I choose circular symmetry (after clearing all other symmetry) then the entire bottle changes...I only want to apply symmetry to the top T-spline sections, not the entire bottle.  I tried selecting those top sections and applying symmetry, but the circular symmetry grows to encompass/changes the entire model.

 

Need answers to these questions:

 

-the top circle lip is not fully circular...how can I make it a circle that will allow circular symmetry to be added to it?

 

-If I have a non-circular symmetric body, how do I isolate that body before applying circular symmetry?  It seems I might have to apply some planar symmetry, isolate the body sections I do not want to change, then apply circular symmetry, but that seems like it is too complex (and what if I had a shape was not symmetric in any way int he forst place, yet I wanted to change one specific area to be internally circular-symmetric?)

 

A:  It sounds like you could sculpt the top portion and lower portion independently with circular symmetry applied to the upper section.  Subsequently you could then bridge the circular symmetry section to the non-symmetric section.  T-Splines will try to maintain the symmetric section while bridging to the non-symmetric body.  You will notice the lower section will be highlighted in red (a terrible choice of color highlight which needs to be addressed).  The faces in this region will be isolated from the circular symmetry.  You can isolate symmetry at any point with the Isolate Symmetry command so you could build the entire model up to the top with symmetry and then isolate the symmetry subsequently to those faces in the lower area.

 

7.png

 

How To Start Guided Tutorials?

Q:  When I opened a new installation of Autodesk 360 Fusion for the first time, there was a tutorial popup with various guided tutorials(like a lamp). I closed the box initially, but would now like to try them. How do I trigger the guided tutorials again? There doesn't appear to be any way to do so in the UI.

 

A:  Try using the Step by Step Tutorials from the Help drop down menu, see below for clarification.

 

13.png

 

Copying objects

Q:  This may be a stupid question - but I need to create 10 copies of an assembly with about 10 components. I am having a hard time. I can't get it to copy and paste a group of components - the option just disappears from the pull down. I'm sure there is a simple answer and I'm fairly new at Fusion 360 obviously. 

A:  There are a couple of ways in which you can get multiple copies of an assembly that are independent to each other.

 

1. In your Data Panel, click on the Projects link to punch out to A360 Web.  Select the assembly and click on Copy from the Action menu.  You may have to do this a few times (first time copy 1, second time you can copy 2 - original + copy, etc).

 

2. Again, punch out to A360 as aboe.  Export your assembly as a Fusion 360 Archive.  You will get an exported copy in your dashboard.  Download the exported .f3d file, make 9 copies on your desktop and upload all of them to your project.

 

If you want all of them in a higher level assembly, you will have to Insert each of the copies into the higher level assembly and position them appropriately.

 

How to create a spline in a Sketch with specific radii / radius

Q:  The Sketch environment is the place for exacting measurements, so I assume there is a way to do this...see the screenshot here:

 

 8.png

 

A:  This is a little notch cut out of the bottom of a liquor bottle.  If you see the slope on the side of the notch, there is never a place that the cutout is ever straight.....a perfect place to define a spline.  At the top of the notch the radius is defined as 2.5mm and at the bottom of the notch the radius is 1mm creating that slope.

 

If you look in Fusion 360 in the Sketch environment, creating a Spline indeed does create nice little circles for you....but those circles have no way of being edited to define a specific radius....how can I define a specific radius to the two ends/generated circles of the spline to get the above slope?

 

9.png

 

Alternatively, maybe I am doing it wrong, but the Spline command certainly seems like what I need, since those circles are automatically created, and (hopefully) just waiting for me to define their radius!

 

It's possible to dimension the curvature arc (using the sketch dimension command), and editing the dimension could change the radius.

10.png

 

Cut text at specific depth across organic curve

 

Q:  Hi all....I have seen other posts on this forum talking about cutting text into regular bodies (spheres, fillets, etc.) but I have need of cutting text into a body that is irregular/organic.  Can someone suggest a workflow for this?

 

What I need:  cut some text at a 1mm depth into an organically shaped body and have the text remain readable

 

I originally though that after I created the text (and exploded it) I could "project" it onto a surface but:

 

-I was unable to do so via the "project to surface" command

-and even if I was able to do that, the slope of the organic body would make the lettering become skewed, and I want the lettering to remain regular

 

Here is an example of the profile of the cutting text via the Extrude command:

 

11.png 

 

...as you can see, the text at the top is cut too deep, and the text at the bottom is not even cutting at all.....I want the text to be cut at 1mm wherever it might touch the body.

 

Just to give another view, here is another view:

 

12.png

 

Can anyone suggest ideas on how to do this?  The above example was created very quickly by Sculpting a box, making the corner irregular, and projecting text....very easy to re-create.

 

The actual use case for this is the modeling of a liquor bottle that is basically an ellipse...the logo of the band need to be cut into the body at a 1mm depth across the face of the bottle, but since it is an irregular shape, just extruding the text will cause the above issue.

 

A:  Extrude the text using the "to" distance
Be sure to change from "join" to "new body."
Then hide the main body, use "press pull" on the curved text faces that were created by terminating to the main body. In the press pull dialog choose, "new offset" and then offset the faces the depth you want to cut into the main body.
Lastly, turn the main body back on and use "combine" to "subtract" the text from the main body.

 

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Message 14 of 22
herzinj
in reply to: herzinj

Here’s the solution roundup from the week ending 9/14.  Thanks for all the help this week from Jon.dean, innovatenate, Jakefowler, Bespenship.  A lot of great Screencast videos and images up there to help with these solutions.

 

Where is all the surface primitive shapes?

Q:  I only have Loft and Patch!  According the learning videos, there are many more options.

 

A:  I think you are on the wrong menu. Take a look at my video; link shown below:

 

View Primitive_Shapes now.

 

Construction Lines

 

Q:  Having come to Fusion from years of Autocad I don’t seem to be able to find the 'construction line' feature.  These were the dotted lines that you were able to draw and move to aid in 2D sketches

 

My work around is to draw regular lines and then have to go back and clean up the mess  Am i missing something here? Do they exist and of so where?

 

A:  I'm not sure if this is what you looking for, but any sketch figure can be converted to a construction figure by right clicking on it in the work space. See the below ScreenCast for detail.

 

 

 

 Ghost vertices on edges distort knot vector (?) but do not add basic spline?

Q:  Another newbie question: I discovered ghost T-points in my model. They correspond to vertices of degree 2: basically, the split an existing edge.

 

 

  1.  Drag (window) selection will not find them. Why?

That's the first surprise: you'd have to put the cursor exactly over their position to get them to show! Is that a bug or a feature??

 

2. They affect the spline in weird ways, why?

Simplified, I have this very simply control box for a T-spline (5x1x1) and I use "insert point" to bisect the edge shown in the upper left. I expect this to asymmetrically influence the rounded end: another B-spline would be added for this T-point, it should tug in the left, upper corner, no?

 

1.gif

 

But instead the effect of the ghost point is symmetric!!!  It seems as if the horizontal knot-vector is hacked somehow, because the vertical edges are now mapped further to the left, in inverse proportion to their horizontal distance from the ghost point. Is that right? And why?

 

A:  1. This is the intended behavior currently: vertices are not picked up by group selections (this applies to solids & surfaces as well as T-Splines). The original reason for this was to improve selection performance; but since then we haven't encountered many cases where it was necessary to include vertices in group selections (since selecting edges will also effectively select their connected vertices). Operations that specifically act upon vertices will show them automatically, and pick them up in group selection. You have identified a good case that proves a disadvantage with this; we can think about whether there's any good solution for this. But currently I think the performance advantages this gives us are worthwhile, and I don't believe we've heard any requests in the past for changes to this behavior.

2. Yes, this is correct behavior, although it is a bit counterintuitive; it's something of a hidden property of T-Splines. It's related to the fact that T-points and star points can't coexist within a small region. If you insert a T-point (such as this) within two faces of a star point, underneath it will effectively propagate invisible edges from this point, until the T-points sit at least two faces away from any star point. In this case, as these hidden edges propagate away from the T-point, they will always be adjacent to a star point, so they will wrap around the whole part and back into themselves. So inserting a T-point here effectively becomes the same as inserting an entire edge ring:

 

2.png

It's this property of T-Splines that can result in edge insertion/subdividing to cause shape changes in unexpected areas of the model. Unfortunately it's an unavoidable effect of the way T-Splines works. [An alternative way to implement this would be to insert these 'hidden' edges automatically as actual model edges; but this would add additional complexity to the model, and might not be any less confusing in the end.] The only way to actively avoid this effect is to make sure you don't insert T-points within a 2-face region of star points on the model. Note that if you use the Exact insertion option (which maintains the smooth shape, usually by inserting more new edges), it will add the additional propagated edges as proper model edges. 

 

Filling gap between 2 components

Q:  I know there is ongoing discussion into sheet metal with fusion so in the short term i have used the following workaround to generate folded sheet metal parts for my project.

 

Now this isn’t to much of an issue in the sketch as laser cutting is 2D not 3D but when rendering my solution leaves a gap that i would really like to fill.

 

My workaround is to extrude the part then split it into bodies and then components but this leaves a section where the material would be stretched in real life missing. So is there an easy way to fill the missing section as seen in the picture below.

 

A:  I think I may have made the inside bend radius too large in the below video; however, you may be able to use the Patch Environment tools to get some surfaces in place and stitched together, add fillets, and thicken last. This could give you an approximate sheet metal part. I made a Screencast to show how I did this, below.

 

 

Strange part movement using Macbook Pro Trackpad.

Q:  When I use my the trackpad on my Macbook Pro, I get strange random rotations. The part will freely spin like it's in orbit mode. Then it will quit and work normally. This happens randomly although it seems like it's when the pointer is in the upper left of the screen. 

 

A:  If you disable (uncheck) the "Use gesture-based view navigation" option in the General panel of the Preferences, does this help?

How do you use parts from one design in another design

Q:  How do I use parts from an assembly/design in another design?

 

A:  Not seeing your data, generally people set up their design so that each part in a Fusion design is a component.  If that's the case, you can right-click on the component in the browser tree and select "Save Copy As" to create an independent part document from that component.

 

If you have bodies and have not created components, you can right-click on the body in the browser tree and either save as STL, or convert to component, followed by doing a "Save Copy As" on the component as described above.

 

New update always getting prompt of a crash

 

Q:  When I opened the older version last night and got the pop up saying there was a update . it started downloading and I got the fusion has crashed window but it kept updating . Now when I open fusion it gives me the crash window , if I put it in the back ground I can use fusion with one problem my files are not being uploaded to the cloud . 

 

A:  I would suggest first trying to re-install since it sounds like an issue occurred during the update. Please try to uninstall Fusion 360 using the Clean Uninstall technique in the below link.

 

http://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How-...

 

Next, download and install a "fresh" Fusion 360 "trial" from the below web page by selecting the Download a Free Trial.

 

http://fusion360.autodesk.com/about

 

Sketch offset loops in combination with mirror not working

 

Q:  I am trying to do the following, I create a rectangle with a chamfered edge (there is no sketch feature for this!?) and then created two lines to mirror it in 2 directions.

 

Upon offsetting, I have to do the square a quarter at a time because offset does not recognized it as a full loop. Even worse, the initial sketch, when offseting will also take the Normal/Construction lines in the offset. Trying to do an individual selection with ctrl does not seem to work, it goed to offset immediately after moving the mouse.

 

Short list of my problems:

- Missing chamfered edge sketch feature (for solids its there).

- Offset feature cannot select a loop created from mirrored sketch entities. Forcing me to repeat this event 4 times.

- Cannot select multiple individual items to offset with ctrl (this is probably user error).

- Normal/construction lines are also offseted. Isn't it the point of these line types that they are not included?

- When selecting a bunch of lines from my sketch and clicking the offset function, everything is deselected and I have to select what I want to offset (again!).

 

A:  For the chamfer command, you should "suggest an idea" in the Fusion 360 Idea Station. This is simply a command that has not been implemented. If you do create an Idea, please post it here and I will add a Vote to it!

 

The offset seems to only pick chained entities versus the true loop. I'm not sure why the offset command will not pick up adjacent, collinear lines as part of the same loop; however, I suspect it has to do with the mirror command. As for not being able to multi-select sketch entities when the Loop Select command is disabled, I think this may be bug. I will both of these items with the development team to be reviewed further. Thank you again for reporting this. I will circle back with further information as soon as it becomes available.

 

For a potential solution, you may sketch out the rectangle without mirroring or patterning it to achieve results that the offset command can use to offset the entire profile. I note that I was able to draw the sketch line for the "chamfer" and than pattern that successfully. If you add a center point manually (sketch point), then add a few sketch points that are constrained to be midpoints on the rectangle, you can achieve a similar effect to mirroring/patterning by using a horizontal/vertical constraint between the mid and center points.

 

See the below image for clarification. 

 

 3.png

 

4.png

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Message 15 of 22
herzinj
in reply to: herzinj

Here are the solutions for the week ending in 9/21.  Thanks for the support from Innovatenate, joel.palioca, herzinj, rishivadher, dennis.ossadnik, and NicolasXu.

 

Orbit problems, Was this changed in new release?

 

Q:  Having all kinds of problems with orbit since I installed the new release.  I've always used the shift key & mouse method but now the model will just suddenly fly off the screen when rotating.  Also, there are times orbit will throw the model off the screen after I've released the shift key and mouse button.  This has all come about with the new release.  Any thoughts anyone?

 

A:  Are you setting the pivot point when orbiting? To do this, hold shift and then press and release the middle mouse button. You will note a small red dot will appear on screen to represent the pivot point. Now when you hold shift and the middle mouse button, you will rotate about this point during orbit.

 

Scaling and anchoring

 

Q:  When we move a body, there is a way to adjust the anchoring and move it according to the new anchor ( i am talking about this one)

 

1.png 

 

but when we scale bodies , such anchor doesn’t exist, and to scale the body from it's own center you have to go through creating an auxiliary body in that center just to be able to pick a point there . Or as in the example on the picture - creating extra geometry to be able to pick that new point. 


2.png

 

I think using the anchoring system from Move with the Scale operation could really improve the workflow.  Is there another way to scale bodies ( relative to their own center or otherwise) ?

 

A:  An option for the Scale "point" field to choose the center of mass/volume would be a great suggestion to add in the Fusion 360 IdeaStation (link below).

 

http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/idb-p/125/tab/most-recent

 

One suggestion may be to use the align command to move bodies to a work point or the origin, which can be used for the "point" selection in the scale command. I've made quick screencast video to demonstrate.

 

 

IGES import

 

Q:  Just a quick question....I uploaded an IGES file into a project...but I don't see how to bring that into a Fusion workspace.....it is just sitting there only allowing me to download it again....I would love to convert it, but I don't see any options to use it in any way besides viewing it online/in the dashboard?

 

A:  It turns out that the iges file was an iges wireframe which will not import.

 

Mesh to BRep...where did it go?

Q:  I cannot see where the Convert Mesh to BRep function went?  I can "create base feature" and import an .STL file that way...but I the convert feature is only available in the "Create Form" environment, and then only to T-Spline?

 

A:  Would you happen to be in a Parametric file, or a Direct?  The convert mesh to BRep option is shown in our Direct modeling environment, or through leveraging the Base Feature option inside of a Parametric file.

 

3.png

 

Make a joint to a specific dimensional point on a component.

 

Q:  I am trying to join the socket in the picture to the outside of cylinder tube at an exact dimensional location.  What is the best way to do this?

 

A:  I managed to get the two pin ends to connect my making a small hole in them to snap a joint to. But this was easy because when you create a hole it picks the center. So this will not work on this occasion, unless it’s possible to tell fusion exactly where to create the hole on the cylinder.

 

4.png

 

I would suggest to create a sketch with a point on the outside of your cylinder tube.

You can apply dimensions to take control over your point.

After that use a joint to fit the pin and the cylinder.

 

I created a video here:

https://screencast.autodesk.com/Main/Details/da97d7e4-5643-4327-b3a6-45778f298fb7

 

How to Snap-to / Move a SINGLE component when multiple copies exist?

 

Q:  I have copied/pasted several identical components and if I use the manual MOVE control for the entire component it only moves that particular component.  But if I try to select a point on an object so I can SNAP-TO / MOVE a component (right click a corner and select MOVE) it attempts to move ALL of the similar components instead of just the one I'm focusing on...   How do I SNAP-TO an individual component?

 

A:  In the Move command, we may use the Point to Point transform to snap the component. Is it what you want?

 

5.png

 

Rotating an SVG file?

Q:  How do you rotate an SVG file?

 

A:  If you are in Direct Edit Mode, you can use the move command to rotate a sketch. You may try right clicking on the sketch in the timeline and selecting Convert to DM feature. Now, edit the resulting Base Feature in the Timeline and you may right click on the sketch in the Browser and choose move. The move triad will have an options to rotate the sketch.

 

Please note that if you have any fixed sketch entities, this may impact the behavior of a move command.  I've a made a ScreenCast that shows how I might tackle this issue, below. 

 

 

Did the Fusion 360 free noncommercial enthusiast option just go away?

 

A:  Rest assured we are committed to personal usage. We simple changed the name of the free option to be more clear (so we thought) to users.

I copied this from the details of the Fusion 360 pricing page:

 

"Are you a startup (a product not yet commercially available) or planning to use Fusion 360 for personal use?

If Yes, you qualify as a Startup.

 

If you selected the startup entitlement, you will have personal use of Autodesk® Fusion 360™ for one (1) year. You will be notified at the end of your entitlement term via email or via a notice to your account. At the end of one (1) year, you will have the option to re-select the startup entitlement of transition to a commercial entitlement."

 

As Fusion has matured, we hear more and more about products users designed and now think might be great product to bring to market. By changing the name to "Start up" we were trying to be more clear that we want and encourage users to make the jump from maker to entrepreneur. 

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Message 16 of 22
kingson138
in reply to: herzinj

Hi James,

 

I noticed that the ability to move Offset Planes to any position had been added to the "Create Form" and "Create Base Feature" environments. But the offset planes have to be constructed in either environment, then they can be moved to any position by selecting the planes and using the "Move" command. Offset Planes  in the  parametric mode cannot be moved in those two environments (Create Form and Create Base Feature) . Only Offset Planes constructed in the  non parametric environments can be moved. After "Finish Form" or "Finish Base Feature" the moved planes will stay at the new position. Offset Planes created in the "Create Form" workspace can also be moved in the "Create Base Feature" workspace or envoronment. The reverse is also true.

 

Kingson

Edited


Regards,
Kingson
Using Apple computers
Message 17 of 22
herzinj
in reply to: herzinj

Here is the solution roundup for the week ending 9/28.  Special thanks to Dunderhead, Kingson138, Joel.palioca, innovatenate, and marshaltu for helping out the community with these great answers.  Keep it up!

 

Mesh to BRep...where did it go?

 

Q:  Very quick question...I cannot see where the Convert Mesh to BRep function went?  I can "create base feature" and import a .STL file that way...but I the convert feature is only available in the "Create Form" environment, and then only to T-Spline?

 

A:  Would you happen to be in a Parametric file, or a Direct?  The convert mesh to BRep option is shown in our Direct modeling environment, or through leveraging the Base Feature option inside of a Parametric file.

 

 1.png

 

Can't get local files to open.

 

Q:  I'm trying to open some locally stored Inventor and STP files in the September release of Fusion 360 and I can't.  When I try to open them, I get the following error message "Opening of local files is not supported!".  How do I get around this?

 

A:  You can upload those files to your project firstly and then you would be able to open them.

 

 2.png

 

Rotate Body around its center

 

Q:  There's literally no way to do such simple thing any 3d package has. Or is there? I cant seem to find a way to rotate a body around its center.. or set center point.

 

A:  Yes we do have the capability to set the center point.  We have some plans to make this more discoverable in the future, hopefully it will be easier to use when that happens.  Below is a video of an example on how you can change the center point so that you can have a different location to rotate around.

 

 

Editing Components of a Feature

 

Q:  How can you edit the components of a feature. For instance, I have a fillet with multiple edges selected and later decide I do not want one of the edges to be included. When I go in to edit the feature how can I add or remove individual edges or components? Same question for drafts, extrusions, patterns, etc.

 

A:  You should be able to control this on mac by holding the command button to unselect or select additional items, for PC this should be control.

 

Force a dialog box (i.e. INSPECT/MEASURE) to remain on-screen @ all times?

 

Q:  I'm constantly glancing @ object dimensions and I have plenty of screen real estate.  I want to keep some dialog box windows open 100% of the time.  Is there a way to "pin" them so they remain open @ all times? 

 

A:  At this point we don't have this capability.  This seems like a great suggestion though, what you can do is you can add your idea to our IdeaStation which allows other users to also help vote up the importance of ideas like this.  These ideas help us to tailor the product for what our users want to have.

 

http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/idb-p/125/tab/most-recent

 

If you see yourself using a command often you do have the ability to add an item to the Toolbar if it isn't already there, this may not solve what you are looking for, but its great for often used commands.  You can do this by clicking the Add to Toolbar button, on the right side.

 

3.png

 

How to alter/change Push/Pull INCREMENT snap values?

Q:  When I attempt to press/pull any object it defaults to .5mm snapping.  How do I change this default snapping increment to something different (i.e.  .25mm)?

 

A:  The snapping increments are dependent on how you have setup your options.  If you take a look at the Layout Grid option in the navigation toolbar at the bottom of your screen you should see a few things there that may be helpful.

 

8.png 

 

If you choose the option to "Set Snap Value" you will be prompted with a couple different options.  One is Fixed and the other is Adaptive.

 

Fixed allows you to set a specific value for each snapping increment.  If you are constantly using the save value this may be useful to you.


Adaptive changes the snapping increment dependent on how zoomed in you are.  The closer you zoom in, the smaller the value gets for snapping.  This seems to be the preferred method since it allows you to zoom in to gain greater fidelity with your increments.

 

API for Fusion 360 available

 

Q:  IS there an API available for Fusion 360 ( and I can investigate the structure, and maybe come up with a solid to t-splines script) .. but also usefull for other purposes of course (a la Inventor)

 

A:  Blog Post: http://modthemachine.typepad.com/my_weblog/2014/09/im-back-and-have-some-fusion-360-news.html

 

Documentation: http://fusion360.autodesk.com/resources

  

Inset edge in parametric mode...how to offset by specific distance

 

Q:  I have a cylinder I created in Sculpt mode with some nice curves to it.  The thing  I am trying to reproduce has a small bump that starts out at 2.5mm below the top.  

 

When I "Insert Edge" I only get a number between 0 and 100 percent, and not any specific distance.  Maybe parametric mode does not support this, but I want to say "Inset edge 2.5mm away from the edge I selected to start the insertion from".  This functionality should not be constricted by the "next" T-sline line...If I need something 2.5mm down the object then that is where I would like to put it.

 

I realize that the Sketch environment allows for precise measurements, but I want to create a beautiful T-sline curve...I just want to start and end it at the right place.

 

I also tried creating construction planes but ran into a couple of problems:

 

-construction planes cannot be offset/selected from a T-spline "face"...I can only select the global plane and figure out the measurements myself

-I cannot snap the "insert edge" command to a plane so I have to eyeball it

-The "Insert Edge --> Offset" functionality does not seem to do anything, even though I can select a construction plane

-The "Insert Edge --> Offset --> Measure" never seems to change...that seems liek what I am looking for but maybe offset is not what I am looking for.

 

4.png

 

A:  Hi to offset a construction plane up and down or to any position is not possible at the Parametric Mode in this version. You have to stop recording to go to Direct Modeling Mode. Then you can go to Sculpt workspace and the construction planes can be moved to any position you wanted. I am not sure if the new update coming on September 2, 2014 will add that capability. I had been requesting that many times and nothing seems to had been done. This is in fact a missing feature.

 

If you are at the  "Create Form" workspace at the parametric mode you have to "Finish form" before going into Direct Modeling Mode.

  

Body/Component in Ghost Mode

 

Q:  What causes a Body or Component to go into Ghost Mode?

 

5.png

 

A:  I played around with the design history a little more and I managed to find the ghost objects at the end of time!  But they were tucked away in the main "Bodies" folder, not in the component in which I was working.  I think that was what tripped me up.  Basically, I think what is going on is that once you go back in time, objects that you created later  (such as breps that are converted T-splines, the stuff you get by "finish form") do not exist, they cannot be edited, yet, they do exist in the future!  That is why you will see the surface appearance, from the future, on a T spline that has already been converted if you go back in time to edit it.  All of this makes perfectly sense as I write it, but it has to be experienced!!!

 

You can disassociate this connection by right clicking on your T spline and toggle "show/hide associated bodies".

 

Click and drag problem in tutorial

 

Q:  During the tutorial there is a step that requires you to click and drag or slide the switch. I cannot get this function to work.

Will you please help me?

 

6.png 

 

A:  Apologies for the inconvenience, to get things working correctly for this tutorial what you can do is disable contact sets prior to the move.  See the image below on how to turn off contact sets.

 

7.png

We have plans to get this fix in one of the upcoming updates to resolve any further issues.

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Message 18 of 22
herzinj
in reply to: herzinj

Here is the roundup of solutions for the week ending 10/15/14.  Thanks to everyone for their continued support on the forums!

 

Daylight Saving Issue

 

Q:  It's Spring here in New Zealand and we've just switched to daylight saving time, clocks go forwards one hour.  Since then Fusion 360 will not start and comes up with an inaccurate error essage saying I need to correct my clock and time zone settings.  I can get it to open as a work around by putting the clock back an hour on my PC, but this is a pain to do every time, and as long as Fusion 360 is in use, all my appointments and reminders on my calendar are out by an hour which is inconvenient.  Would it not be better for Autodesk to correct it's clock for daylight saving once rather than getting customers to do it over and over?

 

A:  You may consider changing from the current Time Server to the NIST Time Server.

 

1. Go to the Start Screen, Right-click to get the "All Apps" icon in the lower right of the screen, and click it.

2. Select "Control Panel"

3. From Control Panel, navigate to "System and Security" >> "Clock, Language, and Region" >> "Date and Time"

4. Click the "Internet Time" tab, and change the server to "time.nist.gov", then click "change settings"

5. Check if the correct time is displayed with the "auto DST option" in (Date and Time tab > Change Time Zone).

 

 

Convert mesh into surface

 

Q:  I present you my problem : I would like to convert a mesh into a surface.

 

The initial file's format is PLY, but I can't open it with Inventor or Fusion 360. With other software that I have, I can convert it into : STL or OBJ.

If I convert it in STL, I could see it : it is tri-mesh. When I use the tool "Convert" there is a message "Warning too many triangles...". I have seen two explications in this forum :

  • "Convert" does not work very well with tri-mesh : so I turn it to Quad-mesh, but it does not work more...
  • This is because it is a STL file and fusion 360 do not like STL files, and it is better to use STP.

I have the same problem with OBJ.

 

So, in my dashboard, when I try to export the STL (or OBJ) to STP, it does not work too... In fact, it works but it is an empty file... And I receive a pdf "Warning your file was empty".

 

A:  You are close, but I think I can clear up a few things for you.

 

Unfortunately there is an upper limit to the amount of data you can feed any CAD program. We have found that Fusion becomes unusable when you open a mesh with an extremely high number of triangles. You have such a model. The good news is you may be able to simplify your file using MeshMixer, which is free.

 

http://www.meshmixer.com/index.html

 

Your second question, about export to STEP or STP, which is a "solid" format, very different from Mesh. Mesh files must be converted before you can export as a solid file. So you can't export as STEP without the conversion, and you can't convert because Fusion won't open a file with too many triangles.

  

Render error

 

Q:  After a few seconds, render mode fails and outputs garbage. MacBook Pro.  The background is black in Fusion.

 

1.png

 

Always the same effect, independent of model or Fusion version (since beta)

Product looks great in A360 though...

 

A:  Unfortunately, the Intel HD 3000 graphics chip set is just not robust enough for rendering. Right now we are working towards graphics certification and it's looking like cards like this may not be supported. Typically for 3D graphics you would want 512 MB or greater GPU memory. The recommended card for Maya on Mac, for instance, is almost a full GB.

 

Things you can try:

Reduce the load on your graphics following these suggested settings:

http://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How-...

 

Also, you could try reducing the window size of Fusion during rendering. Or consider getting a more modern and CAD capable graphics card.

 

How to make a toolpath from a complex STL file?

 

Q:  How do I make a tool path from a complex STL file? I can convert simple STL files to BRep, but my file is too complex and it either hangs or I get the error "This mesh contains a large number of facets. Conversion [spelled wrong] aborted" when I try to convert it to BRep. Is there any way to just make a tool path from the STL directly, without converting it? MeshCAM can do it, but I would like to be able to use Fusion for all my tool path needs.

 

A:  The CAM module in Fusion360 cannot work directly with the STL file. So there needs to be some kind of conversion to Brep or surfaces.  A couple of ideas.

 

1. You might want to simplify your complex STL mesh first with free products like Meshmixer ( http://www.123dapp.com/meshmixer) and then re-attempt the conversion. Maybe you get more lucky this way.

2. If you have access to our 3DS Max product, you could open the STL in 3DS Max then export the mesh to SAT. The SAT file can be uploaded to Fusion and you can use the Create toolpath command directly on the uploaded SAT file. 

 

Finally, once you venture in toolpath territory and if you encounter more problems, I would strongly suggest to post your questions not on this forum but on the dedicated CAM forum at http://camforum.autodesk.com/

 

How to Create surface primitive shapes?

 

Q:  I am trying to Create surface primitive shapes but any without success.

 

I have also seen the video below, but I can not find the surface primitive shapes as shown in the video.


When I am in Patch mode and I click on Create, I can only choose between Pach and Loft. Where are all the surface primitive shapes such as box, cylinder, sphere, etc.?

 

Create surface primitive shapes (See the first 14 seconds):

http://help.autodesk.com/view/NINVFUS/ENU/?guid=GUID-010E380E-7CD2-49F5-ABE6-6BECDB9B2CDB

  

A:  The Patch primitive commands are available while in Direct Modeling (DM) only. You can temporarily enter a DM environment with the Timeline still activated by using the Create Base Feature command in the Model work space > Create drop down menu. I've made a quick ScreenCast below to demonstrate this.

 

 

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Message 19 of 22
herzinj
in reply to: herzinj

Here’s just a ton of solutions from the past couple weeks, ending on 10/19.  Thanks to everyone’s continued participation, especially those going out of their way to provide solutions such as Joel.palioca, Phil.E, Innovatenate, theCADWhisperer and Herzinj.

 

4K monitor Model disappears

Q:  Just upgraded to a 4K monitor (Viewsonic VX2880ml) and using the built in graphics Intel HD graphics on DH77EB Motherboard with latest drivers on Windows 7 64 with all updates. At 1920 x 1080 the part shows up in the view fine (see attached screen shots below) however when I change the resolution to 3840 x 2160 the part is not displayed.

 

A:  At the 3840 x 2160 resolution would you be able to do a quick test for me?  If you reduce the window size of Fusion to something closer to 1920 x 1080 and attempt to open the model again does the problem still exist?  You can do this by opening the program and just click and dragging a corner to a smaller window size.  We are aware of graphic problems with high resolution monitors where the graphics card runs out of virtual memory and as such the model disappears, this is actually a common problem with 3D video applications in general, but we are looking at ways to improve this within Fusion 360.

 

Another couple things to take a quick look at is some of your effect options.  Try disabling all of these effects:

 

1.png

 

And check your graphics preferences within Fusion 360:

 

2.png

 

Fusion model size limitations

Q:  What are the model size limitation on Fusion?  Or at what size model does the software begin to have difficulty with?  Can I model a post frame construction building 20' x 30'?

 

A:  The represented size doesn't matter. I have models that are 1 mile across. Performance only slows due to graphics, displaying textures and all the model interaction highlighting.

 

Pipe feature MAC

Q:  Why does the "Pipe" feature not exists in History-Mode? This affects other Features to.

- Fluid volume

- Find features

- Joints

....

 

A:  Because we have not completed the work to make those commands parametric.

 

Previews black shaded

Q:  I just uploaded about 8 .igs files into a new Project.  When I am in the Autodesk360 online hub and I click on the file to view them in the spinny viewer some of them are nice and white with shadows highlighting them as I spin them around...and some are dark black with some white highlights as I spin them around.  The black models I cannot discern any sort of lines on them, and they are basically not something I can show to others.....does anyone know why this is happening?

 

A:  This doesn't sound like the correct behavior, but I note that I am getting a similar issue. When I upload CAD data to the previews for some file formats appear to be pretty dark.

 

I note that if you find those IGES file in your data panel in Fusion 360, right click on them and select Create Fusion Design, the previews are much brighter since the file is converted to a native Fusion 360 file.

 

 3.png

 

MODEL->CREATE->WEB function

Q:  I am going down the menus, trying out every feature and function one-by-one.

 

So far so good except the Model -> Create -> Web function which I can't seem to figure out. I tried looking for documentation, examples, tutorial, videos but found nothing. Can someone help me understand what it does and how to use it.

 

A:

4.png

 

 

5.png

 

Sketch to construction line menu entry "normal/construction"

Q:  I created a sketch (circle) and want to display it like a construction line.

I saw this in a short video (https://screencast.autodesk.com/Main/Details/1c309551-c6c1-4ff5-aeb6-650d5fac1ba4) but i cant find the menu option "normal/construction" command on MAC-Version of Fusion.  Where can i find the command?

 

A:  Try these steps.

6.png

 

7.png

 

8.png

 

Problem launching Fusion 360 after offline

Q:  I worked offline on my MacBook Air and now I get the following error when I try and launch it. When I click OK, the program loads but quits as soon as I click anywhere.

 

9.png

 

I can launch it fine from my Mac desktop. I can also log in to the web site: https://myhub.autodesk360.com/portal/ on my laptop. I signed into A360 and all it A:  did was create a new hub. I switched hubs but still couldn't get in. Can you suggest something for me to try?

 

There is a options file you need to remove from your problem machine.

 

Go to finder, use go to folder, enter ~/library.

Go to the location below and delete the options file NMachinespecificoptions.xml

 

10.png

 

Start Fusion.

 

2d drawings on MAC

Q:  2d drawings are now not supported on MAC-Version.

Is that a temporarily state and can i hope that this feature is coming soon in next versions (Fusion ultimate)?

 

A:  You are correct. The currently release version of Fusion 360 contains a Windows-only technical preview  for Fusion 360 Drawings. However, in a future release of Fusion 360, drawings will no longer a preview will be available on the Mac OS in the Ultimate Version of Fusion. See the below link for further detail.

 

http://forums.autodesk.com/t5/design-differently/expanding-the-fusion-360-family-introducing-fusion-...

 

 

Loft Command Missing??

Q: Trying to locate the loft Command in Fusion 360.  Not under Create or Modify?

 

A:  It is not yet supported in the history based modeling environment.

Turn off the history recording and you should have access to Loft (right click on the top node of the browser).

 

11.png 

 

This thread demonstrates a couple of Lofted features.

http://forums.autodesk.com/t5/Help-and-Support/Is-a-3D-Sketch-possible-in-Fusion/td-p/5096368

 

How to make inset fillet?

Q:  I am completely new to Fusion 360 and I am trying to follow the lamp example.  In the example there is a slide (15 of 30) that asks you to fillet an edge to 50mm.  When I perform this task the fillet creates a fillet away from the edge creating a ramp (pardon my uneducated terminology).  The fillet is supposed to be inset creating a curve under the edge.  I've attached images demonstrating what it should look like and what it actually looks like.  Can anyone help me understand what I am doing wrong?  

 

A:  I think the problem that you are having is that the part you are trying to have the inset fillet on was not created as a new body.  When you create that part and extrude or push/pull it, if you use Join instead of New Body, it will create the fillet between those joined bodies like you are seeing.  To have it inset, if the lamp arm is a new body, you will be able to make it inset like in the image you attached.  Let me know if this isn't the case!

 

Operation: New Body

 

12.png

 

Edit Face???

 

Q:  I cannot find the edit face function in the model.

 

A:  don't think is will be available in a parametric, timeline document.  If you start a direct modeling document or switch to not capturing Design History you should find it.

 

 14.png

 

Here is what I do. Add a Form feature to the timeline then using the create face command int eh sculpt environment create a set of faces on top of the solid model face you want to sculpt.  Using create face lets you easily lay out the topology like you want.

 

Next using edit form edit the face as you see fit.

 

Exit the Form feature and use replace face to replace the target model face with the source surface you created in the form feature.

 

This creates an editable face that you can go back and edit as often as you need.  This is an example where the timeline allows you much more freedom to makes edits later as your design evolves.

 

 

offset problem

 

Q:  tried using offset to create line after line on this but wouldnt let me do anymore than one.   

 

A:  I made a quick screencast to show the decal and the custom appearance workflow. 

 

Move Manipulator

 

Q:  I'm modifying a face in Sculpt mode, but I don't want to rotate the face from where the manipulator is. how do I move the manipulator itself to center on where I want to be rotating from?

  

A:  You can adjust where the manipulator sits by using the re-orient tool. There are limited options for placement: center of face, vertex, center of edges. Give it a try!

 

13.png

 

Mirror a mirrored feature

Q:  I'm making a bracket to 3D print to hold some screwdrivers in a pegboard. Nothing fancy, just trying Fusion 360. Once again I'm running in to something that I could swear should be super easy but it is apparently not working for me.

 

What I want is to mirror the hook once rather close to it and then mirror both of these over to the other side. For some reason I am unable to select a mirror as a feature, so the last (4th) hook cannot be made by using the original.

 

15.png

 

16.png 

 

A:  Are you using the "pattern features" option in the mirror command? I think my approach may be to only model one-half of the part and then use the "pattern bodies" option to mirror the whole part instead of just a few features. If you share a sample file, I will be happy to take a look at it.

 

 Import dfx issue

Q:  When I import this file I get no errors, but when I open it in fusion 360 no elements appear, the file shows up empty.  Working fine in 2d programs here, what do i need to do to get files like this into 360 correctly?

 

A:  Does draftsight have a command similar to explode? You may try exploding the figures if they are some sort of block. This may convert them to a figure type that is readable for Fusion 360. I'm not sure if this will work, but just a suggestion to try. Let me know if that helps.

 

 

 

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Message 20 of 22
herzinj
in reply to: herzinj

Here are the solutions for the week ending 10/26/14.  Thanks to rishivadher, NicolasXu, marshaltu, schneik, garin, charegb, Phil.E and innovatenate for their solutions this week!

 

Fusion 360 Toolbars

Q:  I accidentally deleted the Render icon from my Render toolbar (it is still in the dropdown menu) and I cannot get it back. How does one modify or customize the toolbars???

 

A:  Expand the drop down in the toolbar menu, each row in the menu has a little arrow at the end on the right. Click this arrow to put that menu item on the toolbar. You can drag and drop to reorder the toolbar, or drag the icon off to remove it.

 

synchronization error; opening .f3d files

Q:  Yesterday Fusion 360 was unable to sync, and so would not let me save my files in the normal manner.  Thankfully I was able to export backups, so the work was not lost, but this morning it still refuses to synch, and thus will not let me open my backups within Fusion 360. 

 

In the data panel a blue bar has appeared under the project name which reads "Fusion 360 synchronization error.  We are trying to refresh."  My internet connection is working fine, and I can log into my A360 account without issue.  The really odd thing is that it does seem to be synchronizing, since files I upload in A360 appear in Fusion, but because Fusion doesn't think it's syncing, I can't save files.  What's more, when I uploaded a .f3d file in A360, although it shows up in Fusion, I can't open it; double-clicking it in the data panel just opens it's page in A360.

 

I'm on a MacBook Pro running OSX 10.9.4 and Fusion 360 2.0.1291.  I've tried logging out and back into my Fusion account, repairing permissions on my disk, and restarting my computer.  No dice.

 

A:  Something may be wrong with your account. Can you log in your hub https://myhub.autodesk360.com successfully? If yes, are there any errors/warnings in your project?

 

Next experiment would be to delete all cache files under "/Users/davidjsher/Library/Application Support/Autodesk/Web Services". You may have to log in again when launch Fusion after that.

 

Is there a way to take the model data and create a 2D dimensional drawing? 

Q:  is there a way to take the model data and create a 2D dimensional drawing? 

 

A:  We just pushed out an update tonight that will let you create drawings in the Windows version of Fusion 360. We are still working on the Mac version and will introduce it in an upcoming update.

 

Basic 2D drawing

Q:  I've just started using Fusion 360 in trial and playing with the 2D drawing beta. While reading through some of the announcements I found that next month, that feature will only be available in the new Premium version. I'm hoping that you will consider leaving a basic 2D drawing/dimensioning in the reduced feature version. As a hobbyist, I don't need detailed cross-sectioned drawings, but a basic drawing with dimensions. I'm attaching a drawing of a peppermill that shows as much if not more detail than necessary. I've used some other programs that can do the design and print a drawing with dimensions, but Fusion 360 makes it much easier to design and make refinements. Anyway, thank you for your consideration.

 

A:  Drawings and CAM are currently tech previews. Both will be graduating and become part of the product.

 

2.5 axis CAM will be in Fusion 360, this includes simulation of 2.5 axis toolpaths

3 Axis CAM will be sold as part of Fusion 360 Ultimate. Eventually ( first half of next year) we will sell it as a module that you could buy al a carte.

2D sketching is in both Fusion 360 and Fusion 360 Ultimate. As you state it is pretty fundamental.

2D Associative drawings is in both Fusion 360 and Fusion 360 Ultimate. There is naturally a bit of confusion on this, as the plan changed in the last week based on user feedback.

 

Enthusiasts and companies starting up can still get Fusion 360 for Free. So you get drawings and 2.5 axis cam as part of the free "start up" license.

 

3D preview is all black in Chrome

Q:  When I view my projects in the 3D viewer online, all I can see using Google Chrome is a blacked out background. It does work in Firefox. It had been working, but I'm using the dev channel which is updated frequently. Anyone else experiencing this or is this a problem with the version of Chrome I'm using?

 

A:  Which OS are you using and what is your graphics hardware? Your link renders fine in Chrome for me on Win 7 using a Nvidia Quarto card.

 

Fusion 360 Questions: Hide Grid & Change Lighting (for Mac)

Q:  For Mac Version Fusion 360:

How does one hide the Fusion 360 grid for a nice snapshot or view without the grid showing (like in 123D Design)???

And how does one change the lighting in a Fusion 360 model (not rendered) in modeling mode???

 

A:  To remove the layout grid display:

 

1.png

 

There isn't a direct lighting control outside of Render, but you may find enough variety by changing environments:

 

 2.png

 

Fusion 360 Question: radius or diameter of circle or arc not given???

Q:  When I create, say, a 3-point arc or circle, it kindly tells me the three points, but not the radius or diameter of the resulting arc or circle as I am building it. I need that. What am I missing???

 

A: For 3 point arc and circle you should apply a dimension afterwards.

 

3.png

 

Convert Projected lines to Sketch lines

Q:  Is there any way to convert the purple projected lines to sketch lines? I thought that I could first generate a series of projected lines by planar cut and then use them to generate a new form using a sketch, but I am struggling.

 

4.png

 

A:  The magenta colored sketch figures indicate that they have been projected. You can highlight/select these figures, right click and select Break Link to turn these into regular sketch figures. By regular, I mean not projected and not fixed.

 

5.png 

 

I'm not sure if that is the command you're looking for, but I hope it helps. You should still be able to use projected figures to create a new form, I think. Please give it a try and let me know if it helps or if there are further questions.

 

sketches exploding when moving axis

Q:  Why do the sketches move when I move a line which is used to project constructin planes along onto which I put sketches?

 

https://drive.google.com/file/d/0Byzv_NlyKp_2ZFNXSHNmMHZvWUk/view?usp=sharing

 

A:  This is a problem solved by using projected geometry to relate the driving curve (the long line) to the downstream sketches.

 

In your video, when you move the line, the downstream curves are only attached to the plane. They are not attached to the position of the line within those sketches.

 

In order for the downstream sketch to remain in a relationship with the driving curve, you must project the driving curve into the sketch and dimension or constrain to it. This is a common workflow in parametric modeling, such as Fusion or Inventor.

 

The reason the sketch slides away in your video can best be likened to parallax error.

 

https://screencast.autodesk.com/Main/Details/be100d2f-f9ec-4ea8-aa41-c7488ef9a6c8

 

basic help - measurements

Q:  I just downloaded fusion 460, so I know very little. 

Is there a way to change the size of a box AFTER it was created to have a particular (different) size  (a matter of changing a measurement); and is there a way to create a feature on the box (e.g., a shaft) that is anchored to a specified point on the box (a slightly different matter of measurement)?

 

A:  Thanks for asking the questions. Re-anchoring during Press/Pull might be useful for the intent. Please refer to the video below for steps:

https://dl.dropboxusercontent.com/u/73595450/PressPull_ReAnchor.mp4

 

Apparent bug in Selection?

Q:  I find that if I marquee select (with select through checked, and going left to right) and touch another object with the selection rectangle, that object becomes selected when I subsequently choose the Move tool. This seems like a bug. 

 

https://screencast.autodesk.com/Embed/Timeline/b2db89d4-71cf-4a70-9d68-2baafb43eb0b

  

A:  You have discovered an as-designed feature. The selection window you draw in the video completely surrounds an edge on the small box body. This selected edge is promoted to a Body selection for the move command. This way you can just click an edge of a body, right click, and pick Move, thus eliminating the need to do window selections moving single bodies.

 

999.png

  

Sketching on face

Q:  When creating a sketch on a face of a model if appears to project all the cut edges as pink lines.  Can they be used as geometry/  if I need the edge should I trace over them?  Can I trim them if needed?  I assume if I change the underlying model they will update?

 

A:  Yes the purple edges are auto-projected.
They are associative, so you can use them and snap to them and they update if the model updates.
To trim them you can RMB on the sketch curve and "Break Link" this then makes the curve a normal curve that behaves just like any line you draw.

 

Rib Web workflow ???? confused with direction

Q:  How does Fusion understand what direction to grow the rib / web ? I was able to do it on one side  the second side the tool fails to understand the direction.

 

one side wored:

 

 6.png

 

other side does not

 

7.png

 

A:  The cursor hint for the rib command reads:

 

" Uses an open sketch curve to create a thin feature. The rib is created planar to the sketch plane."

 

For this reason, I suspect the rib command is working as designed. A better example of what one may use the rib feature for is below. Note that sketch 16 (the sketch selected in the Rib command) is located on Plane 4 (visible in the workspace).

 

8.png 

 

I suspect that the command you are looking for in this instance is the web command. The cursor hint for the web command reads:

 

"Uses an open sketch curve to create a thin feature. The web is created normal to the sketch plane."

 

If you use the Web command and disable the Extend curves on the really "angled" web sketches, it seems to help. I suspect there is some limitation in the extend option that is preventing those two webs from solving. I will submit this to development for further study.

 

9.png 

 

Please let me know if you have any questions or concerns. I hope this helps.

 

One other note I wanted to make is that if I offset the sketch to be below the "top" of the part the web command will work with the extend option enabled. Hopefully, the below screen shot helps to clarify what I mean by this.

 

10.png 

 

The reason it work well on one side and not the other is that the sketch is located "above" or outside the extents the body. See the below image and let me know if this make any sense.

 

11.png

 

Besides isolate/hide, any other way to avoid this?

Q:  So I come across this nagging problem that I have with Fusion 360, how do I cut a sketch/profile without affecting other components that intersects it? I know that isolate or hide that component that is intersecting will avoid it but why do it still affect other components that is supposedly not active?

 

12.png

 

13.png

 

A:  You have to "Suppress" the bearing our the object that is between the model that you have to cut, then "Unsuppressed" to have the result

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