Deconstructing a Solid Assembly

[Anonymous]

I received an IPT from the manufacturer of our cold saw; an IAM was not available.  What are some good resources for learning how to deconstruct the IPT into a working assembly?  The end goal is to be able to simulate the saw with work-piece fixtures.

[Mark.Lancaster]

@Anonymous

ALthough this article https://synergiscadblog.com/2015/11/23/inventor-icopy/ is for iCopy workflow, flow steps 13 through 15 to make an assembly and parts from your part model.

[johnsonshiue]

Hi! You can simply use Make Components command to push individual solids to individual parts. Please note that each solid will result in a unique part. For shared parts (multiple occurrences of a part like a bolt), you will need to use Replace Component command to swap out the unique parts. Then, what do you want to do after that?

Many thanks!

[Anonymous]

This may be the way to go.  I'm working on it when I have time for now.

So like the bolt example, this procedure applies to mating parts? In the attached capture, all of this is in Solid1, which seems daunting at a glance having never done this before.

I think for the purpose the only objects I will need to keep are the saw head and vise base, removing the rest.

[johnsonshiue]

Hi! I am sorry I am a bit confused. I thought you had 18 solid bodies. Why all of a sudden they become one solid?

Many thanks!

[Anonymous]

I can understand how I may have confused you, sorry about that.

Yes, the provided model has 18 solids, originally in STEP format, but 95% of the design was in one solid, as shown in the image below.  This is where the deconstructing comes in, creating the necessary components off of what is provided and creating a proper assembly.

[Frederick_Law]

You'll need to copy the ipt file and use sketch and extrude to remove part of the solid to get parts you need.

You maybe able to use delete face but it depends on how the solid is.

If you can attach the STEP file, we can check it out.

[johnsonshiue]

Hi! You could decompose the bodies within Solid1. It is not a popular workflow but it is doable. Right-click on Solid1 -> Repair Bodies.  You will enter Repair Environment. Unstitch the whole solid. Then use Transfer Surface command to move faces to Composite nodes. It is like grouping the bodies. After a few iterations, you will be able to make more solid bodies out of Solid1.

Please try it out and see if it works for you.

Many thanks!

[TheCADWhisperer]

It could be a simple matter of what Options were set when opening the STEP.

A user with experience translating STEP could probably provide much better diagnosis with the actual *.stp file.

[WHolzwarth]

Looking at your picture and seeing only one solid visible with several nested parts, I'd suggest copying to Construction environment, unstitching and quality checking there, and creating new solids after re-stitching from there.

If it's a STEP from Solidworks, I'd expect several missing internal faces.

But it's not hopeless ..

[Anonymous]

I revisited the emails with the design engineer and he had first sent me an IPT for 2019, but I'm on 2018 still.  I've attached both the ipt and stp files here.

[WHolzwarth]

2019 IPT is a derived component of an Inventor IAM, melted into a single body without any internal surfaces. Not much can be done besides isolating each member, and creating an own part file.

The STEP is better here. As expected, several faces between parts are missing.But repairing seems to be possible in most cases. First result is the black handle at the top left.

[Anonymous]

Nice work!  I'm reading up on the Repair Bodies feature which will take some time and practice to grasp.

If I may ask, what steps did you use to get get the black handle?

[WHolzwarth · Accepted solution]

Short description:

- Copy Solid1 to Construction (CE). Set it invisible in Modeling environment (ME)

- In CE, unstitch Solid1

- Do a Quality check.

- Select faces near the handle and move them to a new group

- Switch Solid1 in CE invisible

- Patch hole at the handle's bottom

- Stitch the group. Result will be a solid and a few rest of faces

- Do a Copy Object with this solid. Result is another body in ME

- Same procedure for the next candidate

[Anonymous]

At first it's a bit cumbersome but it gets the job done.  Thanks for sharing your knowledge.

[WHolzwarth]

  No success without some sweat before ..