Cannot retrieve dimensions from extrude in derived part in assembly

[mikeb456]

I make a simple revolved part = part1

Derive another part = part2 from part1

add a hole and an extrude to end face of part2

put part2 in an assembly grounded at origin

make a drawing of the assembly and create a view of the end face with the extrude and hole in part 2.

Try to retrieve dimensions from the hole and extrude in part2 but I can only get the hole diameter not the extrude dimensions.

As attached.

Any help or confirmation that this is a bug very welcome.

thanks Mike

Inventor Pro 2017 Build 233

[TheCADWhisperer]

Try this -

In the part file mark the desired parameters for Export.

In the assembly file Link to the part file and select the desired parameters.

(Actually, you can do this in one step from the assembly as Inventor will automatically mark selected dimension for export (and give you notification).

If you also want the Extrusion Depth then I suggest that you give it a named parameter in Part 1 and link all the way through into Derived and Assembly.

[Roelof.Feijen]

There is definitely something strange going on.

If you Suppress the Derived Feature in Part2

Go to drawing and use Retrieve Dimensions, it works for both the Hole and the Extrusion.

Edit: I am not able to reproduce your problem building my own Parts, Assembly and Drawing.

Can you? I am running the same Version / Build on Windows 10.

[TheCADWhisperer]

---

@MikeBundock wrote:
...make a drawing....

---

Oops, I guess I got confused by the thread title and completely missed this part of the problem description.

I didn't realize this wasn't strictly an assembly *.iam question until reading @Roelof.Feijen response.

[mikeb456]

Confirming that if I suppress the derived feature/part I can retrieve the extrude dimensions too. Odd.

and ... if I delete the retrieved (while derive suppressed) extrude dimensions and un-suppress the derived part the extrude dimensions return to being non-retrievable.

ref reproducibility ..

I found the problem in some live parts I'm working on so created the basic drawing/assembly/parts that I posted with the OP to check the behaviour.

I've also tried sharing the extrude's sketch, making it visible, etc with no effect. Seems suppressing the derived part is the only work around.

Its walking talking and smelling like a bug to me.

[Sofia.Xanthopoulou]

Hi all, 

either I am thinking too flat or I didn't get the point. 

Why would Inventor give you a retrieved dimension if there isn't anyone in the sketch?

The other thing is I couldn't even open the drawing without error message - is there something else in it?

Please watch my video and tell me what I misunderstood.

Regards

[mikeb456]

The dimensions that won't retrieve are in the sketch1 that's consumed by extrusion1 in part2. Strangely the diameter dimension for hole2 in part2 will retrieve. Thanks for looking at this. MIke

[Sofia.Xanthopoulou]

Yes, and if sketch 1 has a dimension, I can retrieve it. In your case neither the sketch nor the extrusion has a value that can be retrieved. The hole is defined, therefore can be retrieved. 

Correct me if I am wrong.

Regards

[mikeb456]

Sketch1 in part1 has no dimensions (I didn't particularly need them in the drawing in this case), but sketch1 in part2 (derived from part1) that adds the rectangular cut has dimensions that won't retrieve.

Other things I found..

1. If I add a sketch + dimensions and extrude to part1 (similar to the extrude that's causing me the problem) the dimensions from this extrude's sketch will retrieve in a drawing of an assembly with part2 included.

2. And if I make a drawing of part2 then all dimensions will retrieve correctly.

[Sofia.Xanthopoulou]

Ah... now I see, ...

Please open Part1 and just redefine the revolution and than try it again. I am afraid this is due to your dataset. Because doing your steps from scratch I cannot reproduce what you describe. Only your data shows this behavior.

Regards

[mikeb456 · Accepted solution]

I recreated my data from scratch and I think I've stumbled on the reason we're seeing different behaviours.

I've attached a new packngo of my fresh dataset that exhibits the problem.

To recap ..

I create part1 ... a simple cylindrical part, a revolve of a sketch.

Create part2 as a derived part from part1.

In part2 on an end face of the cylinder sketch some shapes and dimension them. Extrude the shapes to cut through the cylinder (or add material it makes no difference)

Create an assembly1 and add part2

Create a drawing of assembly1 and create a view on the end face of the cylinder.

Retrieve dimensions on this view.

Note that only some dimensions will retrieve.

The key part seems to be how the dimensions are created in the sketch that is used in the extrude in part2.

Scenarios:

1. Dimension is created by , single click on line and then place dimension - dimension WILL retrieve.

2. Dimension is created by click on line , click on another line, place dimension - this dimension will NOT retrieve.

3. dimension is created by click on point, click another point , place dimension - dimension WILL retrieve.

4. dimension is created by a click on arc or circle, then place dimension - this dimension will NOT retrieve.

other dimensions I've tested but not shown in packngo ..

5. angular dimension created by clicking 2 lines and place - will NOT retrieve.

6. angular dimension created by picking 3 points and place - WILL retrieve.

In the attached ZIP is a screen capture of the sketch with dimensions, the dimensions I've highlighted with yellow were created with 2 line clicks (or 1 in the case of the diameter) these will not retrieve. The other dimensions were created with either 2 point clicks or a single line click and these will retrieve.

Of course the reason I've been struggling with this is that I always place dimensions between lines (scenario 2) , always thought this was more robust and best practice.

Mike

[mikeb456 · Accepted solution]

This issue now has a knowledge network article :

https://knowledge.autodesk.com/support/inventor-products/troubleshooting/caas/sfdcarticles/sfdcartic...

Mike

[Sofia.Xanthopoulou]

Thank you for sharing @mikeb456,

so it was pure coincidence that I couldn't recreate your issue - I just took the "right" way to dimension the sketch 

Please mark your post as accepted solution (maybe your previous post, too) so all readers can benefit from your experience. 

Thanks a lot for this contribution!

Regards