create a derived part using only some features

[Namoi1]

just wondering if it's possible to create a derived part using only some of the features of the base components

i.e. I've got a funny shaped part with a bunch of holes in it, and I need another part with exactly the same shape but totally different holes (location and size)

I know you can do this with the different solids in the part (only use some of the solids) but I haven't been able to figure it out with features, if it's possible at all.

I could probably create one base part (just the shape) and derive both parts from that, but then I've got a part lying around doing jack.

[Anonymous]

my understanding is that in cases like these, inventor somewhat follows cold-hard-reality...

either they both they come from the same blank
or
you have to fill & redrill holes if trying to make part 'b' out of a predrilled part 'a'.

if there will be more variations of this item then rebuild all from the blank upwards, otherwise it's pretty easy to patch holes and remake them in VI

[PaulMunford · Accepted solution]

You could derive through as a surface. Then patch the holes, then use the stitch command to turn it back into a solid.

Our use 'delete face' with the heal option turned on.

[csaba.stupak]

The derived comman derives the body(ies) from the part, not the features which creates the body. You can try to insert your part into an assembly and derive that assembly. In the derived assembly dialog select the Options tab and enable Hole Patching - either patch All holes or based on perimeter. This will derive the assembly including your part body and it also removes the holes from the part. You can edit the derived body after this - add new holes to different place.

Thanks,

Csaba

[JDMather]

Of course the best way would have been to have only the common geometry in the master original and then Derive as needed.

Another option in addition to those already described is to Derive and then Delete Face with Heal option to remove unwanted holes.

[Namoi1]

good work around I suppose, and I'll use it, but it would be nice to be able to suppress certain features in the derived part.

Thanks

[IB55]

I have come across with the same issue and to resolve it I used 2 different workarounds:

1. create a base part (part A) with only features common for all intended parts. Then create derived parts (part B, C, D ....)
2. If you can't do option 1 then Save As intended (or existing) base part (part A saved as Part B). Supress all unwanted features in part B, derive new part C from part B. obviously you will loose the link between part A and part C but it is not a difficult task to re-Save_As part B from updated Part A.

[SBix26]

With Inventor 2022, your problem may be solved.  Model States allows both (or all twenty, for example) variants to be defined in one part file.  You can add the different model states to assemblies and to drawings as you wish.

I haven't explored all the implications and possibilities of Model States, but it makes close variants such as you're describing a simpler management task.  One of the most common "identical but different" modeling tasks in my career was mirrored parts.  Now it's simply done in one file and that's all there is to it (in most cases).

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Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
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