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KimBruns
Posts: 94
Registered: ‎09-21-2007
Message 1 of 10 (345 Views)
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Extrude To doesn't update in Assembly

345 Views, 9 Replies
01-17-2014 08:29 AM

I have the beginnings of a tank asm, I am having problems with the Extrude To or the Between option updating after the width of the tank has been updated.  The floor of the tank is pitched so the height of the Back Wall will change based on the width of the tank.

 

There is a Rule that will change the width an length of the tank.  The length is fine, but change the value of the width and see what happens to the Back Wall.

 

What seems to happen when the Floor (or a Plane coplanar with the floor) is selected as the destination plane Inventor creates a new Work Plane that becomes the destination plane.  When the width of the tank is changed the newly created work planes does not react to the change.  See Work Plane6 in Wall_Back.

 

Can someone please tell me why this works this way and how to overcome it.  I know I can do the Trig and put the formulas in the parameters of the wall height but I thought this one of the benefits of parametric modeling.

 

Much Thanks,

 

Kim

 

 

FrontView 5in Chan 1.JPGFrontView 5in Chan 2.JPG


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Valued Contributor
Mario428
Posts: 99
Registered: ‎03-20-2013
Message 2 of 10 (298 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 03:46 AM in reply to: KimBruns

Doing things like that is the appeal of parametric modeling.

Unfortunately Inventor does this very very poorly.

 

The easiest and best way to do a tank in inventor is to model a core that is the inside shape of your tank.

Then make all outside parts adaptive to the core.

 

You can make very substantial changes to the core and the adaptive parts will follow the changes very well

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JDMather
Posts: 26,315
Registered: ‎04-20-2006
Message 3 of 10 (293 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 03:52 AM in reply to: KimBruns

I always use the Copy Object command when editing in context of assembly to get the surface to be used for termination,

but I recommend using multi-body solids techniques instead and then pushing out the assembly.

Please mark this response as "Accept as Solution" if it answers your question.
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Valued Contributor
KimBruns
Posts: 94
Registered: ‎09-21-2007
Message 4 of 10 (280 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 05:05 AM in reply to: JDMather

Thanks for your quick responses guys.  I am just learning to use Inventor and I will give both methods a try.  I have already built a Multi-Body version and a Skeleton version.  I know I had the same problem with the Skeleton version, I don't think I had the problem with the Multi-Body version, I don't remember it's been a month or two since I did it as a Multi-Body.

 

It's seems strange that Inventor (being a somewhat mature product) cannot do what is seemingly a simple process.  Is this not what you'd expect from a parametric modeler?

 

Does anyone know why Inventor creates a Work Plane that becomes the extruded to plane when you selected a solid to extrude to?

 

Autodesk, why does this happen?

 

Thanks,

 

Kim


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JDMather
Posts: 26,315
Registered: ‎04-20-2006
Message 5 of 10 (270 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 05:40 AM in reply to: KimBruns

KimBruns wrote:
It's seems strange that Inventor (being a somewhat mature product) cannot do what is seemingly a simple process.  Is this not what you'd expect from a parametric modeler?

For whatever it is worth - I took a look at your assembly and couldn't figure out the logic of what you were trying to do.  I would have done it completely different.  It struck me as an unconventional technique.

Please mark this response as "Accept as Solution" if it answers your question.
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Valued Contributor
KimBruns
Posts: 94
Registered: ‎09-21-2007
Message 6 of 10 (259 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 06:05 AM in reply to: JDMather

Thanks JD, but could you be more specific instead of denigrating what I did, I was asking for some wisdom.

 

Why is a Work Plane created ( which doesn't update ) when I Extrude To a solid?

 

Thanks,

 

Kim


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JDMather
Posts: 26,315
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Message 7 of 10 (249 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 08:06 AM in reply to: KimBruns

I don't have time to reproduce technique I would use, but it would involve Copy Object as indicated earlier.

Maybe someone else can come along and provide an example.

Please mark this response as "Accept as Solution" if it answers your question.
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Valued Contributor
KimBruns
Posts: 94
Registered: ‎09-21-2007
Message 8 of 10 (235 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 08:51 AM in reply to: JDMather

Thanks again JD for your time and help.

 

As I said earlier, I am just learning and am trying several methods to see what works best for what I'm trying to do. 

 

Back to my question,  I found out that if you constrain the Inventor generated WP and make it coplanar with object that was originally picked, the Extrude To works updates properly.  But this is a ridiculous work around, so I will try another method.

 

Thanks,

 

Kim


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Curtis_Waguespack
Posts: 2,821
Registered: ‎03-08-2006
Message 9 of 10 (225 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 09:10 AM in reply to: KimBruns

Hi KimBruns,

 

I just skimmed through this thread, so I might have missed some important details, but here is something to look into. If you go to the Tools tab > Application Options > Assembly tab, and look for the In Place Features section, you can set the Mate Plane and/or Adapt Feature options to help with you goal.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

Autodesk Inventor In Place Features.png



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Valued Contributor
KimBruns
Posts: 94
Registered: ‎09-21-2007
Message 10 of 10 (208 Views)

Re: Extrude To doesn't update in Assembly

01-20-2014 10:24 AM in reply to: Curtis_Waguespack

Thanks Curtis, I will give it a try.  BTW, I bought your Mastering Inventor 2013 last fall, it is my goto reference. 

 

Thanks again.

 

Kim


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Windows 7 Professional x64
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