Learning - How to Create Solid Extrude from DWG file?

[Anonymous]

Hi, I'm trying to take this 2D sketch to a 3D model.

I figure it would be easy enough to do one of the two methods below, but I'm learning that may not be so.

Method 1 - Trace over all lines somehow to ensure proper dimensions. This saves time not having to re-do the sketch from scratch. Extrude as needed.

Method 2 - Import the DWG file to Inventor. 'Clean up' lines by connecting them. Then project/extrude the sketch.

Method 3 - Re-draw the entire thing from scratch but using Inventor.

Which approach do you recommend? Now onto the errors:

I focused on method 2 - importing the DWG and the import came in nicely.

When I projected, then extruded the outline for the sketch, I could only get a 'hollow' extruded outline. I'm not sure how to fill it as a solid. But I'm confused that the extrude didn't make a solid object in the first place. Can anyone help with this? I'm thinking I just need to draw it from scratch in Inventor...

Update: I added the DWG file. I used the sketch doctor but I can't seem to connect the lines together. I manually dragged the lines together to make them connect, but when I did an extrude, Inventor gave an error saying I couldn't extrude. I forgot the exact error. I'll try to duplicate it, but at this point, I'm thinking I just need to re-draw it. Any help would be amazing. Thank you.

[SBix26 · Accepted solution]

No question about it: my recommendation is Method 3.  Connecting points is one challenge, but so is the possibility of duplicate lines, fudged dimensions, and zero dimensions, to name a few.

Modeling from scratch allows you to completely understand the model, to make use of symmetry where it is useful, and to avoid packing too much into individual features.  Experienced users advocate for the KISS principle when it comes to sketching-- keep it simple.  In general, one feature per sketch; fillets and chamfers last; holes made using Inventor's hole tool, rather than extruding.  There are exceptions to all of these, of course.  The goal is always a robust model that is easily modified as the design evolves.

Note: you forgot to mention what version of Inventor you're using.  It matters if someone tries to help by supplying a file or recommending a workflow that you can't access.

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Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
LinkedIn

[imajar]

Can you get the source file as a 3d object like step or iges?  That would save alot of time and eliminate chance for Error.

One issue you will have no matter what method you use is that the drawing is not fully defined.  For example:  The curved bottom (or top?) is not fully defined, what is the wall thickness, etc?  etc.  I have come across many many drawings in the past where things are not to scale and the only thing you can trust are the written dimensions.

Otherwise, if you know it was drawn to scale then you should be able to model it accurately.  In that case, I think you would be time ahead to just make it from scratch.  (although, for a few things, you might have to import the dwg anyway to get certain details, for example if the curved bottom is a spline shape).  You have already noticed that trying to work directly from the dwg geometry can have some challenges.

[Anonymous]

In my opinion it depends on the use of the model. My preferred way is to redo it in Inventor using best practices so that I can retain design intent, something that is almost as important as the geometry. About the only time I copy straight from AutoCAD is to laser cut something that was in 2D that just needs cut-and I have no other use for the model. Remember, design intent is key!

[jrobrador19 · Accepted solution]

Hi there,

I tried to do Method 2 as well. Here are my inputs.

- The dwg file is not made properly. Whenever I import the dwg file, it prompts that it is not from a licensed Autodesk program. The problem with this file is the lines are not coincident which is the reason why it cannot be extruded as a solid.

-I tried to import only the geometry needed for the extrusion. Since the numbers aren't needed, I tried to select the drawings. It seems that the drawings are linked together which makes you select them all.

-Next, I tried to extract the possible constrains. If constraint are present in the dwg file, it can also be imported. I did this to extract coincident constrains hoping that the lines will be connected.

- The extrusion still can't be done. So what I did is, I tried to use Sketch Doctor but since the dwg file is so bad, it also failed. Sketch Doctor can apply coincident constrains and close loops. 

- I applied coincident constrains to the points of the lines. Using the extrude command, I was able to pinpoint what regions are needed to be fixed. Finally I have extruded it.

Recommendations:

- I think the best way to do this is to edit the dwg file in AutoCAD to be able to close the sketch properly.

- Method 3 might be faster.

I hope this helps.

[JDMather · Accepted solution]

Edit: I see that  @jrobrador19 posted the same findings while I was typing...

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@Anonymous wrote:

Which approach do you recommend? Now onto the errors:

I examined the original geometry in AutoCAD - and it is rubbish.

Normally you could Import (with coincident constraints)

Create some sketch blocks...

... position the blocks relative to the Origin ...and you are off to the races.

[Anonymous]

Yes, that's very true. I was wondering what the thickness of the wall was as well, then referred to the other drawing (the 'lid') and that didn't have it either. So I guesstimated based on a certain dimension at 0.085 inches for wall thickness.

Thank you for taking the time to review!

[Anonymous]

Oops, I'm using Autodesk Inventor Professional 2020

Built 373, Release: 2020.3.3 Date: Thu Sep 17, 2020

Hmm, okay, I will continue to build it from scratch (started to) using those principles. I appreciate it!

[Anonymous]

Quite true. Unfortunately I don't have a 3D source file as this was drawn by 'hand' entirely apparently. I believe in Visio?

[Anonymous]

I'll definitely try this method right now.

If it doesn't work, I'll continue with the from-scratch method, too. Thanks for your prompt response and the screenshots! Very helpful.

[Anonymous]

Wow, awesome! So your recommendation might be to still build from scratch I imagine?

[Anonymous]

Update: So I went ahead and drew it from scratch and it wasn't so bad. But now

1. I'm wondering if I stacked the procedure/steps properly.
2. I want to create that recess to hold a printed circuit board. I'm thinking to do the recess by making a sketch that matches the inner dimensions of the box (ignoring the stubs), then extruding downward to 'cut' the material. Is this sound or is there a better way?

[Anonymous]

Hm, so my dimensions were wrong in the previous model. Here's an updated version

[SBix26]

Here's one way to do it, Inventor 2020 format.  As others have pointed out, the drawing is really badly done: some dimensions missing, many duplicated, some just plain wrong.  AutoCAD reports that the top is an ellipse, so that's what I used for the shape.

There are lots of different ways to tackle this, and mine doesn't really take into account the part(s) that attach to it, simply because I don't have them.  But looking at different people's models is how we all develop a bigger and better toolkit for creating our own models.

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Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
LinkedIn

[jrobrador19 · Accepted solution]

Hi again @Anonymous 

Yes, it seems that recreating the sketch in Inventor will give you a cleaner sketch. The DWG file is to bad that some curves are composed of two curves not tangent with each other and you are not sure if the lines are perpendicularly constrained with each other (in which you will still have to do it).

I think what you're doing for the circuit board is right. Use extrusion to cut out a slot for it.

I hope this helps.

[Anonymous]

This was pretty helpful, too. I tried to build those items in this order described.

[Anonymous]

Wow, this looks amazing! I'm totally reproducing the steps for this on my own, so I can learn how you did it. Then I'll finish build the lid with it. Thank you thank you thank you!

[Anonymous]

Awesome awesome. Thanks!