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RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 1 of 18 (351 Views)
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Workflow question

351 Views, 17 Replies
02-05-2014 11:01 AM

I'm uncertain on how to proceed here, at least efficiently. 

 

Here's the scenario:

 

I have a variety of objects of different sizes going into a foam filled case. The foam consists of several layers. In this instance there are 7 layers, 2 inches thick or thereabouts. I have the objects arranged in a way that the fit in the smallest footprint possible, and so that they are balanced inside the case. 

 

Each object has a sketch drawn, at the part level, of the 'footprint' of the object. This is the cutout that will get cut into each layer of the foam, creating a hollow cavity for the object to sit in. 

 

My conundrum though, is how to do this in the most efficient way possible. as this is something we do here at my company on a regular basis. 

 

In Solidworks (cue eye-rolling), I would have simply picked each of the sketch profiles here in the assembly level, extruded each cavity down through the layers at the varying depths which they require, and choose whether or not I want the feature to show up at the part level. At this point I'd be done with this operation, and on to producing the 2D drawing and exporting die files for the mill to cut. This is not possible in Inventor.

 

Currently, I have to create another sketch here in the assembly level using Project Geometry to select the profiles I need to extrude. I have to do this over and over for each of the different depths I have to extrude. It would be handy if sketches were shareable in assemblies, not sure why it isn't. In this instance, I'd have to create 3 new sketches for each of the three different depths. God help me if I have to revise the outline, because it might not cascade correctly to the new sketches I have to create. After the additional sketches are created, I can extrude through the layers of foam. As you all know, it won't show up at the part level of the foam, so I have to use the Feature Migrator in the app store to push those extruded features to the individual layers. If a change is required to the outline at this point, it is a huge hassle. I'd have to go to each individual foam layer part and delete the migrated feature, then in my assembly, unsuppress the original extrusion feature, delete it (taking care not to delete the sketches along with it) and do the process all over again. As you can see, frustration can run really high. 

 

So my prognosis is, either Inventor is sorely lacking in some of it's "parametric" abilities, or I am missing some sort of work flow that would make this process so much easier. I have posted a pic of the assembly below so that you all can get a better idea of what I'm talking about. Post up with your answers and suggestions!

Screen Shot 2014-02-05 at 1.17.27 PM.png

INVENTOR 2014 STANDARD
IOSX and PARALLELS
*Expert Elite*
JDMather
Posts: 26,161
Registered: ‎04-20-2006
Message 2 of 18 (343 Views)

Re: Workflow question

02-05-2014 11:06 AM in reply to: RDG3PO

Derived Component might be your easiest technique

or

Edit part in context of assembly, Copy Object - surface and Sculpt

or

Mutlibody solids master modeling techniques and push out the assembly.

 

I think there is an add-in somewhere to push assembly level features to part level, but as that is not correct technique in my opinion, I have never tried it out.  Edit: Upon closer read - I see you have found the add-in.

 

Post your assembly here if you can't figure out technique 1, 2 or 3.

Please mark this response as "Accept as Solution" if it answers your question.
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Curtis_Waguespack
Posts: 2,775
Registered: ‎03-08-2006
Message 3 of 18 (332 Views)

Re: Workflow question

02-05-2014 11:23 AM in reply to: RDG3PO

Hi RDG3PO,

 

This video might give some ideas:

http://www.youtube.com/watch?v=6JpK2bEJP-I&list=PL35F652F420934D61&feature=share

 

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



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Active Contributor
RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 4 of 18 (322 Views)

Re: Workflow question

02-05-2014 11:33 AM in reply to: Curtis_Waguespack

Curtis_Waguespack wrote:

Hi RDG3PO,

 

This video might give some ideas:

http://www.youtube.com/watch?v=6JpK2bEJP-I&list=PL35F652F420934D61&feature=share

 

 


Hey Curtis, thanks for posting the link. I'm familiar with it, and it has helped, to a degree. But our facility doesn't 3D mill the foam, its cut out from a profile, and the layers of foam are stacked to provide depth. If we ever upgrade to a 3D milling operation, this is the method we'd probably use, except it requires that the foam layer and the object be in the same part file, which means, doing a lot of copy/subtract bodies operations, considering we've put as many as 30 objects in a billet of foam that's comprised of 7 layers. 

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Active Contributor
RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 5 of 18 (318 Views)

Re: Workflow question

02-05-2014 11:40 AM in reply to: JDMather

JDMather wrote:

Derived Component might be your easiest technique

or

Edit part in context of assembly, Copy Object - surface and Sculpt

or

Mutlibody solids master modeling techniques and push out the assembly.

 

I think there is an add-in somewhere to push assembly level features to part level, but as that is not correct technique in my opinion, I have never tried it out.  Edit: Upon closer read - I see you have found the add-in.

 


I've read that Derived Component would solve my problems before, but I can't find a solid example  of how that works and apply it to our function. 

 

Editing each foam layer in context, copying objects, and subtracting. I'm exploring that option as well, except I have 7 layers and 6 objects. Thats 42 times I have to do that set of commands. That would be doable if I could subtract the objects from the foam assembly itself, but borderline absurd if I have to subtract them from each layer of foam.

 

And I have never heard of "Mutlibody solids master modeling techniques".

 

I will gladly post up the files and would love your help. I just have to make sure that I have nothing in the file thats proprietary first. 

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Curtis_Waguespack
Posts: 2,775
Registered: ‎03-08-2006
Message 6 of 18 (317 Views)

Re: Workflow question

02-05-2014 11:40 AM in reply to: RDG3PO

Hi RDG3PO,

 

Would you be able to create the stacked layers in one part file as seperate solid bodies, and then cut them all at once, and then use the Make Components tool to save out the stackd layer as seperate parts?

 

Make Components

http://www.youtube.com/watch?v=iDRotf2Is2g&feature=share&list=PL35F652F420934D61&index=2

 

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



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cwhetten
Posts: 1,051
Registered: ‎09-03-2008
Message 7 of 18 (311 Views)

Re: Workflow question

02-05-2014 11:48 AM in reply to: RDG3PO

If I was starting this project from scratch, I would use a multi-solid modeling approach.  However, if I had to retrofit an existing model, deriving would be the way to go.  I have attached a simple example of how the derive method would work (at least, one of many ways to do it).  Take a look at it, then post back if I need to explain any of the steps I took.

 

Cameron Whetten
Inventor 2014

Active Contributor
RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 8 of 18 (294 Views)

Re: Workflow question

02-05-2014 12:31 PM in reply to: Curtis_Waguespack

Curtis_Waguespack wrote:

Hi RDG3PO,

 

Would you be able to create the stacked layers in one part file as seperate solid bodies, and then cut them all at once, and then use the Make Components tool to save out the stackd layer as seperate parts?

 

Make Components

http://www.youtube.com/watch?v=iDRotf2Is2g&feature=share&list=PL35F652F420934D61&index=2

 

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


Hey Curtis,

 

We've tried that function too, and I thought it worked well because we didn't have to predetermine the number or thickness of each of the layers till after the cavities had been subtracted from the whole chunk of foam. We opted to use the "bottom up" method so that we could pre place all the foam layers in a template drawing and have them generate automatically. But that's proving to be fruitless anyway because once I use the Feature Migration tool, it likes to generate new copies of the foam layers anyway, for reasons unknown. 

 

I hate to sound like a broken record, but all my problems would be solved if I could share sketches at the assembly level, sharing part level sketches with the assembly. 

 

Thanks for your help though Curtis, the back and forth has been helpful.

INVENTOR 2014 STANDARD
IOSX and PARALLELS
Active Contributor
RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 9 of 18 (289 Views)

Re: Workflow question

02-05-2014 12:49 PM in reply to: cwhetten

Hey Cameron,

 

I checked out the files you supplied, and although I was hesitant to click on the file named "thingies", I'm glad I did!

 

I see how you have all the thingies as one part file, which I understand. Is this a derived component? Some of the placement of the objects in a case is trial and error. Often we have to go back and tweak the location of a component so that it won't interfere with castors, or becasue the cavity needs to be a bit wider, or maybe further away from another component. Would this require making a part file every time the locations of the components were changed?

 

Also, were the individual layers pre-made as parts and placed into the assembly?

INVENTOR 2014 STANDARD
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Active Contributor
RDG3PO
Posts: 43
Registered: ‎07-21-2006
Message 10 of 18 (276 Views)

Re: Workflow question

02-05-2014 01:32 PM in reply to: RDG3PO

Here's a pack and go of the files I'm working with. 

The objects are multibody. The idea is the outer body would be the shape of the cavity, or the envelope of the part. That solid would be hidden once the model was provided to the customer so that they could see their product in th case. 

 

 

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