Sketch Function Needs a Little Tweaking...

[Anonymous]

I am having a blast with this program and appreciate you all very much. That said here are a few items that need looking into.

1) I like to use the left side of my screen, but for some inexplicable reason, when I choose Center Circle, and try to place it on the left part of the grid, the cursor will either not go there at all, or it will hesitate for so long that I give up. If I merely move the screen (hold down center mouse button) and get the area away from the left side of the screen, it works perfect. 

2) This is more workflow related. When I want to move a line I create... lets say its a 2 inch line and I want to move that line over 1/2 inch the Move function will not let me move the line because its somehow anchored to another previous sketch. I cannot figure out how to merely move a line or a rectangle! It either wants to move everything, is anchored on one side, or SOMETHING to prevent me from JUST MOVING THE DARN LINE! All I want to do.. is move an object, unimpeded, from one place to another. I feel more than know that it has something to do with relationships but I am CERTAIN I do not care about relationships at the time I am laying a straight line or rectangle on the sketch. I will concern myself with proper anchoring after I am sure it is exactly where I want it. 

So in review, pull up a design and try to run a line across it. Now click on that line and try to move it. Moving and Copying are so important and I think the flow of those two features could be improved.

3) When using the American standard system in fractions..  When I go to making a box that is 1.75 inches square, then press/pull to 1.75 inches. Now make another box and this time choose 1 3/4. The boxes will not be EXACTLY the same size. They are about 1/128th off of each other. Very small difference but could have a very big impact. ALL of these issues I am having could be JUST ME. So if that is the case, let me know.

4) When making bolts I use the Create Thread function. If I want to Chamfer the end of the bolt so it will go into the hole better, the chamfer messes up the threads (on a 3D print). What is the proper way to chamfer the bolt end? The two YouTube videos that are for that purpose are wrong. You cant just select and chamfer. Not using a 3D printer anyway.

That is all for now, but I want you to know I am loving this program and I am looking forward to the fixes. Your staff really seems to get on this stuff quickly and I have been impressed with the speed at which fixes come out. Thank you!!

[TheCADWhisperer]

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@Anonymous wrote:
...So in review, pull up a design and try to run a line across it. Now click on that line and try to move it...

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I don't think I have ever had the need to "Move" a line.

Can you attach a file and screencast showing your workflow?

[etfrench]

1. Can you do a screencast showing this.  If there are other sketch geometries close to the screen edge, the cursor for a center circle will attempt to align with that geometry and may not move closer to the edge.

2.  Unfortunately, Fusion 360 creates constraints automatically even when they are not needed or wanted.  My workaround when moving constrained geometry is to make and position a copy.  Otherwise, you have to find and delete the constraints. But it's better to use dimensions and parameters to precisely place geometry.

3. A screencast would help.  Press/Pull is (usually/sometimes/maybe) relative to the original surface.

4. McMaster-Carr is your friend.

[Anonymous]

I do not know what a screencast is.

What does my favorite bolt supplier have to do with the making of a bolt in Fusion 360? I am not disputing there is something.I may want more or less chamfer or a different head design than McMaster offers. All I am saying is, simple chamfering doent work, so I am hoping there is a way to do this.

There is something funny about how it seems to want to self anchor on things it has no business self anchoring on. I will do some research on this screen cast thing and submit these issues. I REALLY appreciate your time. 

[HughesTooling]

Here's a thread I made a while ago with a workaround for chamfering thread. One note it doesn't work with threads with a filleted form on the tip, BSP for example. For a BSP thread you'll have to use a sketch and revolve cut.

Mark

[TheCADWhisperer]

Cosmetic first, then toggle the Modeled thread.

http://screencast.autodesk.com

[jeff_strater]

The reason why the line will not move is most likely that you have started the line on the origin point.  This is a fixed point in a sketch.  If you had created the line anywhere else, Move would work as you expect.  But, @etfrench is correct:  Usually one would  use dimensions to precisely position sketch geometry.

Regarding the left hand side of the screen:  You are probably running into the browser.  Though you should be able to place sketch geometry in any area where the browser does not specifically cover.  So, yes, a screencast would be helpful here.  You can always turn off or collapse the browser to get more screen real estate

Jeff

[PhilProcarioJr]

@Anonymous

You can also turn off automatic projection of edges in your preferences, that would solve a lot of your problems, but will not solve the issue if you click on the origin.

[Anonymous]

Thank you all for responding. I find this group very helpful. Here is the new news!

1) Screencast has a bug in it or I am not able to figure out the controls, but whenever you hit Record, the cursor that follows the Center Diameter Circle goes away and turning off Screencast gets it back. So much for Screencast. Let me know if there is something I am doing wrong. In the mean time, just open a new project, Create Sketch, Center Diameter Circle, and watch the cursor that follows behind it. Move your mouse from the far Right of your screen to the far left. If it behaves like mine, it will stop and not allow you to place it anywhere near the Left side. With the Browser disabled or enabled, no difference.

2) THANK YOU for the Bolt information. The idea of choosing the thread but disabling 'Model', making your chamfer, then enabling 'Model' in the thread dialog box solves the problem. Seems a little counter-intuitive to me because I cannot imagine anyone not wanting to model the threads at any time. In 3D printing anyways, Cura (the Slicer) will not slice the threads without Model enabled. But I have a fix so I am happy.

3) I cannot find anywhere in preferences to disable automatic line connections, so that problem is still something I think the programmers can do better on. I go to the origin because I want the exactness TO the origin that it provides. But then I want to move off that model to its mating model and use that line to begin its mate. I am not interested in having to first measure the line so I can then re-create it more inexact somewhere else then move it. Somehow, allow us to stop anchoring! I am used to printed publishing software where we have something called Step and Repeat. It allows us to draw a line, then repeat that line X number of times, X distance (X,Y) apart. Moving one or any of those lines is a matter of grouping/ungrouping. Something for the powers to think about. More flexibility in the Sketch process.

4) Still have the inexactness in the measuring system with a 1.75 inch square box not being the same as a 1 3/4 inch box. What happens if you mix them is, when you press/pull something, the surfaces to not mate together causing a lot of problems. I will avoid mixing them, but just pointing it out.

We made a lot of progress here and I am very thankful. Why is screencast not allowing the cursor to show? 🙂

[TheCADWhisperer]

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@Anonymous wrote:
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2) ... I cannot imagine anyone not wanting to model the threads at any time. In 3D printing anyways, 

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Perhaps for 3D printing.

But if you model an assembly of any appreciable size having modeled threads rather than cosmetic threads will bring your computer to its knees, begging for mercy.

And when (if) you do 2D drawings - for small fasteners the lines for the thread geometry will be so close together than it will be a big black blob of ink.

It is common practice in all of the major MCAD programs to show most threads as cosmetic textures rather than true modeled threads.

[TheCADWhisperer]

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@Anonymous wrote:

4) Still have the inexactness in the measuring system with a 1.75 inch square box not being the same as a 1 3/4 inch box. What happens if you mix them is, when you press/pull something, the surfaces to not mate together causing a lot of problems. 

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All of my models are the dimensions that I specify, nothing more, nothing less.  (Your #3 is not something that I have experienced.)

Can you attach a *.f3d file here that exhibits this characteristic?

[HughesTooling]

I don't see any difference creating a box using press pull or entering dimensions.

[TheCADWhisperer]

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Devek wrote:

1.)... ...Create Sketch, Center Diameter Circle, and watch the cursor that follows behind it. Move your mouse from the far Right of your screen to the far left. If it behaves like mine, it will stop and not allow you to place it anywhere near the Left side. 🙂

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Turn on your sound.

[PhilProcarioJr]

@Anonymous

Hold down the Ctrl key when your drawing stuff and it wont make any constraints.

[Anonymous]

I am not making this up! Here is a poor quality movie I just shot so you can see it for yourself. ScreenCast doesnt work with this problem as the cursor goes completely away when I try to use it. This happens on both of my computers. One is a laptop the other a brand new high power build with the latest graphics cards. There is just no putting a center diameter circle in that area. It is the entire left side. Thanks for going to all the trouble. Also, my 1.75 vs 1-3/4 issue cleared up after I chose the highest decimal resolution in preferences. I do not dispute that some of this has to be me.

[Anonymous]

Thread Modeling ... I am not sure why they would be so literal about it though. For screen and cpu usage, let it show a lesser version of itself. But does it have to BE a lesser version of itself until you check the checkmark? This causes chamfering problems (any type of modification problems) as well as printing problems unless you know the secret to check the model box. This is a super great program and I am merely suggesting maybe there is a way to improve the implementation. The 3D printing applications will not print the threads at all unless modeling is selected. Why? Did I not say I wanted threads on that particular model?

[davebYYPCU]

Default cosmetic threads, you ask why, 

3d printing is the new kid on the block, compared to lathes mills and other machinery existed before cnc came along,

the developers had a 50/50 decision, the default does not create a performance issue, no brainer,

tick the box.

[jeff_strater]

Holy crap, @Anonymous, you are correct (sketch points blocked from the browser area).  I was all set to prove you wrong.  Your movie helped prove me wrong.  I can reproduce the same behavior.  The sketch point input stops at the browser border all the way down, but (at least in my experiments so far) only if you invoke the command from the top toolbar.  If you access the command by the "c" hotkey, or from the marking menu, this does not happen.  Or, if you collapse and expand the browser, the problem also stops happening.  I will log this bug.  Thanks for reporting it.

Also, you are right - screencast prevents recording the problem (I think because it is tracking mouse events).  However, like a good ghost-hunter, I was able to record the bug by using Jing, then recording the replay in screencast...

Here is the bug in action, along with ways to avoid/fix it:

Jeff

[HughesTooling]

@jeff_strater If you promote a sketch tool to the top panel it works correctly as well, it's only a problem picking from the dropdown menu.

Mark

[Anonymous]

I am just thankful we have proactive ghost hunters! Thanks for working the problem!