Imported parts not showing up in idw files Inventor 2019

[perry_a_gray]

I am trying to import parts from places like Mcmaster.com and others. I use to import as a sat file but Inventor crashes when I try. I am now importing as an igs file and it comes in ok. I then save as a native ipt file.When I insert it into an iam I can see it but when I put that iam into an idw file the imported objects are not there. They are visible in the iam but not in the idw. Funny thing is that if I make a base view in a separate sheet of the imported part, it shows up fine. When it is part of an iam assembly it does not show up. How do I undo this invisible part feature and get back the inferior visible parts LOL.

Another issue I am having is when I try to mate these parts to other parts, it always puts them upside down. The surface arrow is always pointing into the part not away from it. So when I mate the part it is inside the part I am trying to mate to. I used to be able to flip this in the constraints window but that does not work.

See attached zip file. Wheel should be attached to the beam. Wheel is visible when it is the base view. If you want me to load a patch give me instructions on how to do that. Pretend I have never done it before which for the most part is true.

[Mark.Lancaster]

@perry_a_gray 

First go to Inventor, Help/About and share a screen shot of Inventor about screen..

Update:  It appears you are still on the original release of Inventor 2019.   Update through manage.autodesk.com/product updates if you're entitled to updates.

Also the info (caster) is surfaces.  So in the drawing you have to right mouse click on the assembly in the given view and say include all surfaces.

[SBix26]

IGES would be just about my last choice for an import format.  I suspect that the imported parts are coming in as surfaces, and surfaces with their normals "inside-out" (though I've also seen that happen with solids). 

I think McMaster Carr creates their CAD models in Solidworks, and I have always had best success with importing Solidworks models from them.

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Sam B
Inventor Pro 2020.2.1 | Windows 10 Home 1903
LinkedIn

[JDMather]

Can you Attach the original IGES file here for experimentation.

The ipt you attached is of a Composite Surface Body.

This is easy to fix (see Attached), but first I would like to experiment with the IGES.

[perry_a_gray]

Build 136, release 2019, Date 2/15/18. Why does it import as a surface instead of a solid? Can I change that?

[JDMather]

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@perry_a_gray wrote:

1. Build 136, release 2019, Date 2/15/18.

2. Why does it import as a surface instead of a solid? Can I change that?

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1. http://Manage.Autodesk.com  and https://knowledge.autodesk.com/support/inventor/downloads/caas/downloads/content/inventor-2019-updat...

2. Zip and Attach original IGES file here.

[perry_a_gray]

What is the file extension for Solidworks files? Attaching IGS. Always use .sat in the past and it worked but this version might have a bug in it.

It won't let me attache the IGS file.

[perry_a_gray]

Here is a link to the caster in Mcmaster.com. Download the format you prefer.

https://www.mcmaster.com/9949t97

[mcgyvr]

@perry_a_gray  In your drawing file edit the base view and go to the "Recovery Options" tab. Check the "Include Surface Bodies" option.

Voila... 👍

[johnsonshiue]

Hi! It is pretty simple to show the surface body in the drawing view. Edit the assembly drawing view -> Recovery -> check Surface body. It was unchecked by default, since most users create drawing views for solid parts.

The composite surface in the part cannot be stitched into solid bodies because there are overlapped surfaces. If you get the STEP file, it should import as solids.

Many thanks!

[perry_a_gray]

Ok, I figured it out. Thanks for the video. I need to load the update. Constraints don't act quite right or at least different than they use to be. The autopredict is turned off. I have more problems with constraints than anything on creating assemblies. I thought that I could flip which side that I mated to in the older version. That function is there but does not do anything now.

[JDMather]

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@perry_a_gray wrote:

 Constraints don't act quite right or at least different than they use to be. ...

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Can you create a Screencast Recording of the trouble you are experiencing with assembly constraints?

I am certain that there is an easy remedy.

[perry_a_gray]

I will create a new post when I have time to work through it. I will try to download the update soon.

[perry_a_gray]

Ok, I downloaded the patch and the constraints are actually working again like they are supposed to. I can get those imported Mcmaster parts to work correctly. Before no matter what I did they were upside down and they would not flip at all. The patches are why I don't update but every two or three years. There is always a patch cycle so once I get through that, I just leave it be. Also, updating versions seems to be a pain now that you have to download it.