Newbie Question about sketching box section frames.

[Anonymous]

Hi all getting back to trying to learn Fusion more and wondering how to achieve what I am after with Fusion.

Situation is I would like to sketch -model box section frames that I weld together for friends to use as dog cages on ute trays and no one item is the same.

Can I use Fusion to create the frames with the driving parameters to allow changes on the fly as a whole model or can i just use it to sketch 1 plane? 

I have attached a file of 2 sides of a frame spaced apart that is a rough idea of the shapes I am after, on the left and right view there will be doors to match the angles.

On the front view I need driving parameters for the bottom bar, uprights, angled pieces, and top bar. Is this achievable as a full 3d modeled part or should i stick to sketches?

[laughingcreek]

Yes, you can absolutely do that.  If you base all your geometry off your sketches there shouldn't be a problem.

one note though: changing parameters in a sketch can produce in predictable results if your sketches aren't fully defined.  Put in enough constraints (dims etc.) so that all your lines turn white indicating, they are fully constrained.  

[laughingcreek · Accepted solution]

instead of doing a copy past of the body that is your frame, copy the whole component. 

[Anonymous]

Great thank you I will try that and get back to the basics. Could I trouble you to look over my next atempt?

[laughingcreek]

of coure, keep posting.

[Anonymous]

Ok didn't take long to get off track again.

Task at hand is to connect the 2 base frame components with a driven parameter for the width between them.

As I have drawn the width bars as a separate component is this achievable with a joint command?

As well as a new component of the door linked in to match the faces of the base frames and spaces as the frames are driven.

 So when I define the dimensions of the base frames the door height-angle updates and then dimension the width bars the base frames expand apart and the door width updates as well?

Seems awfully complicated but I think its achievable with enough crashing around the programme.

[laughingcreek · Accepted solution]

You can do everything you just described.  Might not be worth the trouble for one off, or low numbers of different setups, but as a learning exercise it would be worth while.

For positioning, you are correct, you would use joints.  The trick is to place the joints at geometric locations that are them selves controlled parametrically.   The joint will need geometry to attach to, usually and edge, point, midpoint, etc.

2 ways to go about laying this all out.

-first way (probably the way I would do it) Create a master sketch in the upper level of the design (not in a component) that lays out where every thing goes.  Like a floor plan.  Put construction lines with driving dimensions at locations where components need to go.  When you place components a these locations with joints, the components will move with the sketch.

-the other way would be to place sketches on each component (with the component activated so the sketch goes with the components) that gives places for the joint to connect to (Don't need the sketch if there is already geometry to attach to)

Just want to check, are you aware of how to use user parameters?  Go to "MODIFY/CHANGE PARAMETERS" (looks like a sigma symbol).  Here you can define your own parameter values and use them in when creating sketches and features.

I attached a sample of ONE way (of the hundreds of ways) of creating the door component.  I only defined 3 user parameters for this, but more should be added probably.  open up the user parameters and change the values, you'll see the door shape change.

[Anonymous]

Great thats quite straight forward I will try the master sketch idea out as well.

In your model how was the last extrude defined?  

[laughingcreek · Accepted solution]

For the third extrude, change the "Start" condition to "From Object".  For the "Object," select a face at the end of the previous extrude.

[Anonymous · Accepted solution]

@Anonymous

As @laughingcreek said ;

"For the third extrude, change the "Start" condition to "From Object".  For the "Object," select a face at the end of the previous extrude."

However, to make it clearer for you I have attached a screen shot of what you need to select in order to complete the operation.

In the EDIT FEATURE BOX:

For PROFILE: Select the face in the picture (in Blue)

For OBJECT: Select the upper right face of the extrusion. Second picture

Hope this will help

[Anonymous]

Ahh great I will do some drawings and run through all the features of the pop up menus as I never remember all the options they contain and I never use them as they should be.

[Anonymous]

Glad to hear it helped.
Just make sure to use the correct dimensions in the EDIT FEATURE BOX

If you haven't done it yet, I highly recommend you go through the instructional videos for Fusion360 either on the Autodesk site or in YouTube.if you don't mind asking, what is your experience with CAD/CAE and if so what other platforms have you used?

If you need any help don't hesitate to contact me.

Good luck!

IK

[Anonymous]

Yea I will do that. Thank you for taking the time to help out. My experience is limited to not a lot. I work at a sign shop and had the opertunity to take over the cnc router and laser engraver. So 6 months of heavy youtube and internet searching I am self tought cnc operator. I have had some sketching and asembly with solidworks and use signlab and enroute to run the work jobs through.Watched NYCNC on youtube and saw Fusion and have just been teaching my self from then on. 

[Anonymous]

Wellll took a few trials but got a few solid hours behind a decent computer and I am getting closer!!

The timelines look a bit horrible but the parameters are doing what I am after. So chuffed! 

Thanks again.

[Anonymous]

@Anonymous

Glad to hear you are getting closer and you are chuffed!!! 

I will go through your design and will get back to you with suggestions and help.  The good thing is that "You did it!!!"

Being that you are a newbie, I believe it will be important to get your designs done properly (if there is such a thing ) from the beginning.

If you don't mind me asking, what computer system are you using?

Take care and I will get back to you after I review your design.

Regards,

IK

[Anonymous]

@Anonymous 

I will try to get back to you today.

[Anonymous]

Thanks!My computer system is a new one bought 4 days ago AMDchip 3.2ghz 12gig ram 2Gig graphics. A big step up from my last sys10year old self built setup.The bigest thing was the upgrade from 14" screen to 27" loving it..i can see without squinting!

[Anonymous · Accepted solution]

@Anonymous

Great that you have a much newer computer.  It will make a huge difference with your work!

I got some time to look at your design.  IN reality, for a newbie you did a pretty good job.

However, may I make some suggestions?

>  You designed your BOX thinking as a draftsman (a drawing) and not as complete assembly.

>  I would recommend you create Components and then make an Assembly from them.  Use the power of Fusion for your design functionality and analysis, not as a drafting program.

>  If you want to create working drawings, BOM's, easier mods, etc it would be much better if you would do a design based on Components and then an Assembly.

>  For example, the doors should have a Rotate Joint. Instead of copying and moving from one door to the other you could create a door assembly with 2 instances and Join it to the frame with the correct Joint.  That way you can visualize the functionality of the BOX and make the correct assembly for the door.  You are missing a pin or hinge to make it rotate..

These are just some suggestions.  Try to think as Components that you will put together, not a drawing that you look at that resembles what you want.  The idea of CAD/CAE is to design a product as close as what you are going to manufacture/assemble.  Otherwise, you could had done this with any DRAWING program.  The concept is not to think any more as a drawing that you are looking at but the true Assembly that you are going to build. IMO

Would you like for me to redo the BOX as an assembly with components based from your drawings?  If that helps you I will be glad to do so.  Just let me know.

BTW, have you noticed that Fusion has had Cloud accessibility problems for over 8 hrs. Some components are still not up nd running. i.e. Cloud based Simulation.  Fusion still shows a YELLOW dot on the Job status icon.  For hours we had no access to our data.  

Regards,

IK

[Anonymous]

Yes I ran into the Fusion problems last night. It doesn't affect me that much as I'm just using it as a learning self training platform. Eg: all my experience with gcode was from drawing simple shapes with depth and outputing cam and then going through the code while looking at the simulation. So with what your saying about the box I should be looking at building it like seperate components and then using joints to define components locations?
If your able to give me a demo model of what your describing that would be great.!As long as its not putting you out.
On another idea with the doors of my design, can I draw a sketch in 3d with angle of 32 degrees and extrude as a complete unit? I have scratched trying to sketch in 3d as my atemps have ended in frustration. It sounds like a clean way to do the job but the how to is the trick.Thanks again for your time.

[Anonymous]

Hi,

>  So with what your saying about the box I should be looking at building it like seperate components and then using joints to define components locations?

Yes, the correct way to design is to create components and bodies.  Now, you must remember that only Components can be Joined to create Assemblies.

I went through your drawings and although you achieved what you wanted I would say that they need a lot of refinement.  You need to understand better how to use constraints to lock your drawings and at the same time create parametric relationships.  Parametric relationships are not only set by dimension/formulas but also by the way you use your constraints within your drawings.

By looking at your design it was impossible for me to tell what type of extrusions you are going to use to build the box.  I assume you are going to use square tubing and weld the joint, correct?

If that is the case then it is critical that you define your entire Box model with components.   You need to get the right lengths and end angles for each component in order to fabricate these components.

Regarding; "On another idea with the doors of my design, can I draw a sketch in 3d with angle of 32 degrees and extrude as a complete unit? I have scratched trying to sketch in 3d as my atemps have ended in frustration"

Yes, if you are only doing it as a drawing you can do it.  Here are the steps:

1. Draw on a plane a side view (cross section) of the door (the vertical and 32' angle) with a width of 32mm. You could actually Project from the side of your frame to get that sketch done.

2. Extrude that section to the full width of your door.

3. Using the extrusion you just created you will need to create a sketch on the face of the door with the offset that  you want.  The idea is to create a rectangle on the face of the door to Cut (Extrude) all the material you do not want. You will end up with a frame.

Give me a few minutes and I'll send you the file showing you how to do it.

BTW, please let me know how you plan to build this so I can create a model for you.

Regards,

IK