Part disappears in Isometric View of Drawing

[vanairuser]

Ok. I am a pretty experienced Inventor user. We use 2010. I have a part (it was probably imported as a STEP file some time ago). It is a ball bearing. When I put it in its subassembly drawing, it shows up okay in my exploded parts view of my drawing. But when I use this subassembly in a higher assembly, it doesn't show the entire subassembly. If I delete the bearing, it shows up. But I need that bearing. Is there anything I can do to make it like the bearing? Any workarounds? It's not a surface so including all surfaces doesn't help. I tried toggling its visibility... But the thing is: It used to show up. When I first created this drawing and for some time after that it showed fine. Now, maybe 3 weeks later, it won't show up. HELP!

Thanks,

Dan

[Anonymous]

2 thoughts:

Is the drawing view set to be associative?

and/or is it using a Design View Rep that has it turned off.

or is the IPN using a view rep that is set to not show the part?

[vanairuser]

Okay. I only have one presentation in the IPN. And the subassembly is shown. And I toggled the associativity just in case and it didn't show it still on the drawing. I guess I could always try to download a new bearing file.

[Anonymous]

in your translated IPT version of the bearing, do you have 9 seperate solids?

Or is it all one solid?

It shouldn't matter either way, but if I recall correctly I resolved an issue of this type, by selecting all of the solids, and then right-clicking and using the Copy to Construction option. Then delete all of the solids, then expand the Construction folder and select the solids and rightclick and choose Copy Object, and choose all as a single solid. Not sure if that'll do anything, but it's worth a shot.

also you might attach your IPT of the bearing, for inspection.

[vanairuser]

Ok, I'll try that. The bearing is an assembly with 9 separate solids in my subassembly. 

[Anonymous · Accepted solution]

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@dannyramirez11 wrote:

Ok, I'll try that. The bearing is an assembly with 9 separate solids in my subassembly. 

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I don't quite follow, do you mean:

An assembly file with 9 seperate IPT's?

Or an IPT with 9 separate solids?

either way here is the translated part as a single body IPT, you might try and use Replace Component command to swap out what you have with this file. I'd ground the file you have first and then just delete the broken constraints that will likely result. Then either leave it grounded or unground and re-apply constraints.

[vanairuser]

I created a derived component and made my .IAM into a .IPT and that worked. I replaced my .IAM with the .IPT and then fixed my constraints. Then in the drawing I had to update the view and the subassembly reappeared! Yay! Thanks! I hope this can help someone else in the future!

[Anonymous]

In the future when you go to open the STEP, you may want to click the Options button and choose to import the file as a single IPT file rather than an IAM. You can also choose to do so with or without seperate solid bodies.