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Can't reuse sketch in adaptive part

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Message 1 of 21
barnadaniel
4794 Views, 20 Replies

Can't reuse sketch in adaptive part

Hi,

I have an adaptive part which I created within an assembly. I created work planes in this file, based on features in the assembly, and created a sketch on one of these work planes. I used this sketch for an extrusion. then I wanted to reuse the sketch again for another extrusion - normally one needs to select 'Share sketch' from the right-click menu of the sketch, but this is not available. I have already experienced this (random) behaviour, i.e. the 'Share sketch' option missing from the menu. In those case it was ok to make the sketch visible, and then I could use it again. But now it doesn't help. I made it visible, but when I click Extrusion, Inventor wants me to create a sketch, claiming there is no usable sketch. Why?

thank you

Daniel, Inventor 2013

20 REPLIES 20
Message 2 of 21
jletcher
in reply to: barnadaniel

If the sketch was made in an assembly the sketch cannot be shared.

 

 Now if the sketch is in the part and you make is adaptive you no longer can use shared sketch option.

 

But if you turn off adaptive then turn on share sketch after that turn back on adaptive...

Message 3 of 21
swhite
in reply to: barnadaniel

Yes, it is good practice if you do not actually need a part to be adaptive to turn it off anyways. Inventor will set all parts to adaptive anytime you project lines, sketches etc from another part or assembly. If these lines are simply for reference to create a new part and not for use of true adaptivity, i would turn it off anyways. Adaptive parts require extra time on updates and can even cause an assembly to explode (rare occurrance) if you have too many of them. Only if the part MUST be adaptive leave it on, otherwise turn it off.

Steven White
Lee C. Moore, Inc.
www.lcm-wci.com
Inventor 2011
Intel Dual Xeon E31225 @ 3.1 GHz CPU
16 GB RAM
NVIDIA Quadro 600 GPU
Windows 7 - 64 Bit
Message 4 of 21
barnadaniel
in reply to: barnadaniel

Hi,

Thanks for the answers. I tried to follow your suggestion, maybe in the wrong way.

1) Create a box, and put in into an assembly

2) Create a new part within the assembly, on one face of the box.

3) I projected that face of the box into the primary sketch in the part file (see attached file), and created two closed loops at two diagonally opposite corners of the box.

4) extruded one of these closed loops

5) unchecked 'Adaptive' from the menu of the sketch

6) now I could indeed select 'Share sketch'

7) extruded the other closed loop at the opposite corner of the box

😎 I can not switch back adaptivity anymore (as the attached picture demonstrates).

 

Further questions, comments

- Is there any logical reason why it can not be done what I want to do?

- I do want to make my part adaptive (in the real model that I am working on), since it would connect two different parts within the assembly, which can change size and position. So switching off adaptivity is not an option

- I reached my goal by making yet another sketch, and projecting geometry into that sketch (reproducing once more the first sketch basically), and used that for the second extrusion. Why is this double work needed?

 

Thanks

Message 5 of 21
swhite
in reply to: barnadaniel

Can you not project the shapes edges instead of the sketch used to create the object?

Steven White
Lee C. Moore, Inc.
www.lcm-wci.com
Inventor 2011
Intel Dual Xeon E31225 @ 3.1 GHz CPU
16 GB RAM
NVIDIA Quadro 600 GPU
Windows 7 - 64 Bit
Message 6 of 21
SBix26
in reply to: barnadaniel

I can't tell you why it's necessary, but I don't see why it is a problem to create a new sketch for a new feature.  If there is some connection between the two sketches, just turn on visibility of the first one and project the elements you need into the second sketch.  I routinely work this way even when I could use a shared sketch instead.  Keeps the browser less cluttered.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
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Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

Message 7 of 21
barnadaniel
in reply to: SBix26

It is just extra work. In the original sketch it would just be one extra line (I use one larger profile for the original extrusion, and then use a smaller part of it to extrude-subtract from the body, to a smaller depth). 

Now I need to create a new sketch and project all the lines into it. 

It's not a big problem, but if I don't see why something must be done in a difficult way instead of a simpler way, than I start asking questions 🙂

Message 8 of 21
jletcher
in reply to: barnadaniel

Well 1st off next time you ask for help please post the steps you never said you are using projected geometry..

 

 But don't click on the sketch to make it adaptive click on the feature make it adaptive did not have time to test so not sure if it will work.

 

But to give you some in site I would not use projected geometry. I never use it there are many issues with it.

 

There are better ways to do it...

Message 9 of 21
barnadaniel
in reply to: jletcher

Sorry, so far I used adaptive parts only by 'creating' them within the assembly, i.e. using projections of other objects of the assembly into the part's sketches. So for me adaptivity was a synonim for projected sketches. sorry. 

 

btw. why should one avoid using projected geometry in such a situation? I guess the other methods you suggest include creating the part independently from the assembly, with not fully constrained sketches, adaptive extrusions, etc, and then constraining it within the assembly so that the unconstrained features adapt in size/shape. Why is this method better? (understanding the reasons helps to be more efficient in the future)

 

Thanks

Daniel

Message 10 of 21
jletcher
in reply to: barnadaniel

Projected geometry will slow down performance..

Message 11 of 21
barnadaniel
in reply to: jletcher

Ok great, thanks a lot. 

 

Message 12 of 21
Anonymous
in reply to: barnadaniel

Just found it. 
- right click the feature you want to share the sketch -> Properties 
- make sure "Sketch" under "Adaptive" is not selected -> Ok
- now, try to share the sketch. 
I realized it has to do with the adaptive features since some of the sketches allowed to be shared. 
Hope this helps. 

Cheers

Capture.PNG

Message 13 of 21
JDMather
in reply to: Anonymous


@Anonymous wrote:

Just found it. 
Hope this helps. 


You are 6.5 years late!


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Message 14 of 21
Anonymous
in reply to: JDMather

I'm not sure what you mean by that, but I don't think so since there is no clear answer and "solved solution" for this thread. I take it as a funny remark though.
And that's the goal right, to skip all the non-sense and head to the solution. And since this is a pretty straight forward solution of the original question I thought it'll help future "late" guys who's looking for it and come across with this topic.

Message 15 of 21
dan_mar_san
in reply to: Anonymous

Don't care if this came late. Nobody else bothered to answer or give a simple solution like this one before.

Totally useful. Thank you so much.

Message 16 of 21
johnsonshiue
in reply to: dan_mar_san

Hi! This is a long standing limitation in Adaptive Sketch. I vaguely remember there was a reason to block sharing. It was because shared adaptive sketch could interrupt how features are computed. Also, it can introduce cyclic relationship.

When you use Adaptive workflow, you need to make sure you understand what geometry in what component is the driver and who is being driven. You don't want a driver to be driven or vice versa.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 17 of 21

I found a way but it's full of bugs.

 

My example is doing holes from a part_A to another part_B within the assembly.

 

First I create the sketch and project all the entities I'm going to use, then I make the first holes I want, then I turn the sketch visibility on and make the others holes this makes the sketch shared.

Then it's working if you move part_A the holes adjust in part B but the problems start here.

 

You can remove the adaptivity from part_B within the assembly but if you turn it ON it doesn't work anymore, the second problem is when you want your part adaptive but the holes you don't want them adaptive, well you can't turn that OFF.

 

So I think you *shouldn't try to use shared sketches with adaptivity.

 

*kelly.young has edited for clarity

Manuel Campos Costa
Message 18 of 21

Hi! There is another way you could reference geometry from another component within the same assembly. The command is called Copy Object (3D Model -> Modify -> Copy Object). This command allows you to link body geometry from one part to another. After the geometry is linked, you can project the edges as many times as you want.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 19 of 21

I made a mistake in my last post  I was trying to say the opposed:

 

So I think you shouldn't try to use shared sketches with adaptivity.

 

What I'm doing I think it easier than what you say, I project in one skecth all I want (typically clearances/thread holes and dowel holes) then that sketch is only adaptive and not shared, then in the part I project the edges I didn't use in the first projection into another sketch, that way I can have different types of holes and only one sketch linked to the assembly.

 

I used what you said for other kind of things like a cavity (I know in the mold system you have that, but this version is not the professional one).

 

Thanks!

Manuel Campos Costa
Message 20 of 21
ethan.d.joseph
in reply to: SBix26


@SBix26 wrote:

 Keeps the browser less cluttered.


This is literally the opposite of keeping the browser less cluttered - more planes and sketches.

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