Inventor General Discussion

Inventor General Discussion

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nooneinparticular
Posts: 7
Registered: ‎02-03-2012
Message 1 of 10 (396 Views)
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Negative part files?

396 Views, 9 Replies
10-22-2012 09:05 AM

Inventor Pro 2012, in case it matters.

 

Our company might buy a steel slab as a part.

 

I will take that slab part and put it into an assembly for machining.  I would like to try to follow current company policy and capture the machining as a part.

 

For instance, we will bore a thru hole as a port, a concentric cbore for a ring (to be added in the next-level-assembly) and a hole circle for a CL150 or CL300 bolt circle (for studs, to be added in the next-level assembly).

 

Is there any way I can have a "part" that is completely negative features (hole, cbore, circular bolt pattern) that I can assemble to my slab and have the material removed?

 

I'd really like the "negative part" idea, but I'm open to a workflow that uses derivation of some sort.

 

Thanks for any hints you can offer.

I'm not familiar with ProE, but that sounds alot like an iFeature.

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Ryan.Martinez
Posts: 141
Registered: ‎07-29-2011
Message 2 of 10 (391 Views)

Re: Negative part files?

10-22-2012 09:23 AM in reply to: nooneinparticular

Just an idea not sure if it will give you what your after, but you could create the slab with the machined holes ect in it. Then use view representations to hide the stock slab and show the machined slab.

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blair
Posts: 4,309
Registered: ‎11-13-2006
Message 3 of 10 (388 Views)

Re: Negative part files?

10-22-2012 09:38 AM in reply to: nooneinparticular

Look at "Derived" parts if you wish to have a separate part number for each level.

 

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mrattray
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Registered: ‎09-13-2011
Message 4 of 10 (387 Views)

Re: Negative part files?

10-22-2012 09:39 AM in reply to: nooneinparticular

I don't think there is any form of a "negative part", but I'm sure we can come up with another solution if you describe for us what it is you're hoping to accomplish with these "negative parts".

Is it just to be able to show in a drawing both the unmachined slab and the finished product? If that's the case then an iPart would be great for this. Just make one row of the table the machined version with all features active and the other row the purchased version with only the base slab active.

If you want to be able to "drop" this hole patern and c'bore feature into other parts then iFeature is what you're after.

Or are you after something else?

Mike (not Matt) Rattray

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JDMather
Posts: 28,006
Registered: ‎04-20-2006
Message 5 of 10 (375 Views)

Re: Negative part files?

10-22-2012 10:08 AM in reply to: nooneinparticular

nooneinparticular wrote:

Is there any way I can have a "part" that is completely negative features (hole, cbore, circular bolt pattern) that I can assemble to my slab and have the material removed?

 



I suppose you could have a mult-body solid of the material to be removed - then insert into the stock file and Combine - Cut, but I don't really understand the workflow you are after.

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Active Member
nooneinparticular
Posts: 7
Registered: ‎02-03-2012
Message 6 of 10 (366 Views)

Re: Negative part files?

10-22-2012 10:21 AM in reply to: nooneinparticular

Thank you for the ideas.

 

Selective suppression / reps would be rather "weighty" because each slab can have up to 4 ports (thru hole/cbore/BC combination) and each port can take some 6 different forms.

 

I like the idea of an iFeature, but I get mixed up in all of the parent/child relationships.  The thru hole is referenced off of the default datum planes and the front surface.  The cbore is concentric but on the back surface.  The BC seed is a sketch point ref'd off of the thru hole plus an angle off of vertical.  The first hole is a tapped hole on that point and then circular patterned concentric to the thru hole.

 

As you can see, I've isolated as many references to the thru hole as I can, but the front/back surfaces have me flummoxed.

 

If there is a really good iFeature tutorial, I'd like to see it.  The only one I've found is that silly T-slot tut that imports a sketch.  This is 'way beyond that.

 

As for workflow, my designers will be erectorsetting a machine.  They will get something like "use a B model size 5 slab, port 1 will be drill code GH, port 2 will be drill code HR, port 3 & 4 will be blank".  The drill code is a combination of thru hole/cbore/BC pattern and chamfer.  I want to have them bring up the B model size 5 slab and "drop in" a drill code.

 

Do iFeatures go this far?

 

That multibody idea that popped up as I was writing this might be what I'm after.

 

So as to avoid having a huge debate "thing" on this post, perhaps if someone has a reference to an advanced iFeature tut they could share, I'll research that and the multibody idea, then report back what I've found.

 

TIA

Active Member
nooneinparticular
Posts: 7
Registered: ‎02-03-2012
Message 7 of 10 (289 Views)

Re: Negative part files?

10-23-2012 04:47 AM in reply to: nooneinparticular

I was perusing some of the derived part stuff suggested and I remembered exactly what I am after.

 

If anyone is familiar with Creo / ProE, there is a method called User Defined Feature, or UDF.  A series of features are grouped together and any references external to the features are "tagged" when the UDF is created.  Then those features are promted when the UDF is placed on a new part.  The prompted selections resolve all dependancies for the features.

 

Does Inventor have functionality similar to this?

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mrattray
Posts: 2,513
Registered: ‎09-13-2011
Message 8 of 10 (285 Views)

Re: Negative part files?

10-23-2012 04:56 AM in reply to: nooneinparticular

I'm not familiar with ProE, but that sounds alot like an iFeature.

Mike (not Matt) Rattray

Active Member
nooneinparticular
Posts: 7
Registered: ‎02-03-2012
Message 9 of 10 (272 Views)

Re: Negative part files?

10-23-2012 05:51 AM in reply to: nooneinparticular

Thanks for all the pointers.  I had tried iFeatures before, but they did not work.  Now that I am a bit more familiar with Inventor, I can see that it was the pattern I used for the bolt circle that was failing me.  Why iFeatures do not support circular patterns of holes is beyond my ken to understand.

 

Instead of modelling a threaded hole and then patterning it, I sketched a center point and patterned within the sketch.  then I added holes, using the sketch points as centers.

 

The upshot is... now I've got my functionality using iFeatures.

 

I still need some work pretty-ing up the prompts and perhaps tavbling some inputs... but the core functionality appears to be working.

 

Thanks to all for your input.

Active Member
nooneinparticular
Posts: 7
Registered: ‎02-03-2012
Message 10 of 10 (233 Views)

Re: Negative part files?

10-23-2012 10:03 AM in reply to: nooneinparticular

Ah, but alas....

 

iFeatures are only for part files.

 

I'll just have to make it work.

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