Copy Geometry Associativity

[richard_pears]

Hi,

I'm new here to the forum.

My company just started using Inventor.

We transfer from Siemens NX.

I have a few questions, will post them all as separate topics.

One problem we are having is the copy geometry function.

It seems like I cannot copy geometry as a solid body and have the option for it to be associative

I can copy it as a surface or composite and it will allow me to tick associative

But when I click to be solid the option for associative disappears.

Is this just not possible in inventor?

I can still work like this for what I need to do, but I would prefer just to copy solid if possible for then using the combine function to join or cut out the copied geometry. Instead I currently copy as a surface then use the sculpt.

There also seems to be output options when using copy geometry.

1 method create object that works like I say

the second method join to existing doesn't appear to work for me either

when I select 'join to existing' method it allows me to select the input geometry

but it does not allow me to select the output geometry 'existing'

The way I assume this should work is you are in an assembly for example and want to join one part to another to make all thew same part. I activate the part I want to keep and go to copy geometry, method join to existing, select the other part as input geometry and in output geometry select the active part that I want to join it to.

I am open to suggestions as to other ways to achieve what I am trying to do,

I want to join one part to another or take away one part from another.

My company use joining features for sheet metal.

we bring in the standard joining feature which has a male and female body

we add the male body to one part, and subtract the female from the other and this allows you to join 2 plates for example.

[kacper.suchomski]

Hi

Sculpt or Stitch is a good solution.

If you want to perform boolean operations between parts, a better solution would be to Output Reference Part to Modeled Part.

Additionally, check out the multi-body parts.

[Frederick_Law · Accepted solution]

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@richard_pears wrote:

Hi,

My company use joining features for sheet metal.

we bring in the standard joining feature which has a male and female body

we add the male body to one part, and subtract the female from the other and this allows you to join 2 plates for example.

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That will be iFeature in Inventor.

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-C2D08AAD-D86D-4720-96E4-8E0DA7374BE9

[johnsonshiue · Accepted solution]

Hi! Another approach to consider is to leverage Derive workflow. You may build the "tool" as a part. Then derive the part into the target part as a solid body. Use Move Bodies or Direct Edit -> Body -> Move to relocate the solid body. After that, use Combine command to Boolean the bodies.

When the source part updates, the derived part will be updated accordingly.

Many thanks!

[richard_pears]

Thankyou Fredrick,

ifeatures works quite well from my initial explorations.

It will only allow me to select 1 extrusion feature per ifeature. Ideally I would like to include several extrusions (different bodies) in a ifeature. But this seems a possibility for me thanks I wasn't familiar with using this ifeature tool up to now.

This is really good information for me though thankyou! I didn't know about ifeatures.

[richard_pears]

@johnsonshiue hi

thanks for the suggestion.

I have tried this and I find positioning the derived bodies tricky,

I can move and rotate them but difficult to position them exactly in relation to the other components.

do you have any tips for doing this?

If I could get that bit to work well this seems like it would be the best way as its almost identical to bringing components into an assembly otherwise.

[kacper.suchomski · Accepted solution]

Model 3D -> Edit -> Direct Edit tool -> Body (mode snap, rotate parallel, etc.).

[richard_pears]

thanks, I was missing the snap option that does help alot 🙂

[Frederick_Law]

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@richard_pears wrote:

It will only allow me to select 1 extrusion feature per ifeature.

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It should allow as many features as you need.

I have different size SAE port, group of punch holes.

[richard_pears]

@Frederick_Law 

from what I have seen - it seems to me that it will allow you to select multiple features so long as they are in the same plane orientation. But bit if they are extrusions on multiple planes / orientations it wont allow.

if all the holes are on the same plane maybe this is why we experience difference?

I have found that for me deriving the part that I want to bring in might be a easier solution as it just brings in the entire part into another part. but its not quite as user friendly as the I features to position it so its a shame I cant use that in this case.

but thankyou for suggesting, we do sheet metal work so i'm sure this will come in handy for other applications as with sheet often all in on one plane.

[Frederick_Law]

It need a start plane to locate the first feature.

All other features need to reference the first.

Cant you attach ipt of the feature?

[johnsonshiue]

Hi! In terms of relocating the body, there isn't any other workflow than Move Bodies or Direct Edit -> Body -> Move/Rotate. Direct Edit allows the geometry to be snapped to a reference. It might be useful in some cases.

Many thanks!