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Sketch exits upon dimension edit

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Message 1 of 17
csmac2004
2121 Views, 16 Replies

Sketch exits upon dimension edit

Anybody seen this recently? Using Inventor 2012 SP1 on Windows 7, 64 bit. If we go back into a previously created sketch and edit or add a dimension, upon clicking the green check mark to complete the dimension edit, the sketch exits back to the modelling environment, meaning we have to edit the sketch again to continue with other changes. Obviously no big deal if I'm only editing one dimension, but how often does that happen???

This started happening prior to SP1 being installed. I can't seem to find any other posts on this, so I'm wondering if this is somehow a local issue? We have this happening on multiple computers (all with the same hardware specs) in our office. I don't believe it to be a hardware or driver issue, but I am wondering if it is a process issue. For example, we use project geometry a lot, even projecting from other parts within an assembly (non-adaptively). We also work on SAT file models, rather than geometry initially created from Inventor itself.

 

Any ideas would be appreciated. Thanks!

Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
16 REPLIES 16
Message 2 of 17
JDMather
in reply to: csmac2004


@csmac2004 wrote:

 We have this happening on multiple computers (all with the same hardware specs) in our office. I don't believe it to be a hardware or driver issue, but I am wondering if it is a process issue. 


Attach file here that exhibits this behavior - I don't recall ever seeing or hearing this one.

BTW - you don't need to edit a sketch to change dimensions - just have it visible and double click on dimensions (not sure why you would need to add dimensions - wasn't it dimensioned when created?).


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Message 3 of 17
csmac2004
in reply to: csmac2004

Very good point, about editing by visibility only, not sure why I haven't thought of that workflow, doh! As for adding dimensions, I meant adding dimensions to newly added sketch features (which, in that case, would mean I'd have to edit the sketch). Generally, we just need to edit existing, so the visibility option would work (I'll try it, anyways, but why wouldn't it work).

 

I have attached an example file. The sketch for the drain notches is the one in particular, I haven't tested the others yet.

Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
Message 4 of 17
JDMather
in reply to: csmac2004

I couldn't reproduce the behavior you describe, but as a side note -

you can fully constrain undimensioned blocks, for example simply add a Vertical constraint in Sketch37 and the block is fully constrained (in the sketch).


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Message 5 of 17
csmac2004
in reply to: JDMather

Now I'm intrigued as to why you couldn't reproduce it, so maybe there is a hardware/driver aspect to this. I will test this at home then and see what happens.

 

As for the constraining of the block, that is true. To be completely honest with you, this file I gave you is from a project that we are quite behind the 8 ball on so to speak. As such, we are literally taking absolutely every single shortcut possible, down to some underconstrained sketches for sure...

 

Thanks, though, I'll see what I can do about reproducing this on other systems then... Maybe it is a video card/driver issue or something similar.

 

 

Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
Message 6 of 17
JDMather
in reply to: csmac2004

One thing occured to me is you might be accidently gesture exiting sketch.


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Message 7 of 17
csmac2004
in reply to: JDMather

No, that's for sure not it. Either its something with our process (SAT files, projecting) or our hardware or drivers. If it doesn't happen on other systems (like your own), then I'm thinking hardware but I'm not sure. Whatever the cause, it's annoying as heck to be sure!
Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
Message 8 of 17
SBix26
in reply to: JDMather


@Anonymous wrote:
BTW - you don't need to edit a sketch to change dimensions - just have it visible and double click on dimensions (not sure why you would need to add dimensions - wasn't it dimensioned when created?).

You don't even have to make the sketch visible-- right click on the feature and select Show Dimensions, change dimensions as desired, then click the Update button in the Quick Access bar.

Message 9 of 17
-ianf-
in reply to: csmac2004

We are also seeing this. Although not on every part which seems strange. This has only started occuring recently.

As yet I can't figure out a pattern as to which parts do this and which don't.

Ian Farmery
Inventor & Vault 2023

Dell 7550 Xeon E-2276M, 2.80Ghz 64GB RAM
Nvidia Quadro RTX 4000
Message 10 of 17
-ianf-
in reply to: -ianf-

Figured out what our issue was here.

The parts that were exiting the sketches on edits had some ilogic rules in them containing;

 

InventorVb.DocumentUpdate()

 

This was running with a trigger;

 

Any model parameter change

 

The result was forcing the sketch to exit when editing the dimension.

Ian Farmery
Inventor & Vault 2023

Dell 7550 Xeon E-2276M, 2.80Ghz 64GB RAM
Nvidia Quadro RTX 4000
Message 11 of 17
Mark_Wigan
in reply to: csmac2004

Try sp2

best regards,
- Mark

(Kudo or Tag if helpful - in case it also helps others)

PDSU 2020 Windows 10, 64bit.

Message 12 of 17
csmac2004
in reply to: csmac2004

Yes, we determined it was due to our iLogic code as well. Still happens on 2013, obviously, because that's what that piece of code does! 🙂 Unfortunately, we don't wish to alter the code itself so we're stuck with either suppressing the rule during sketch edits (and hoping we don't forget to unsuppress it after) or just dealing with editing one dimension at a time... 😛

 

Scott MacDonald
Inventor 2013 Product Design Suite
Vault Professional 2013
Windows7 x64
Autodesk Inventor Certified Professional
Message 13 of 17
Baishihu
in reply to: csmac2004

I have the same problem.

 

thanks,

Baishihu

Message 14 of 17
JDMather
in reply to: Baishihu


@Baishihu wrote:

I have the same problem.

 

thanks,

Baishihu


You have not provided any information useful in diagnosing the problem.

What Inventor version (including Service Packs and Updates)?

What Windows OS?

 

Screen captures?

Example files? 

Anything?


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Message 15 of 17
Baishihu
in reply to: JDMather

Thank you for your questions.

 

I believe that was beause of the iLogic. I will study it at my office tomorrow.

 

Regards,

Baishihu

Message 16 of 17
M.Jenaban
in reply to: csmac2004

Hi Scott, 

 

We have had a similar issue. 

 

The solution lies within your iLogic rule/s. If you have triggers (for instance change dimension y when parameter x changes) this can trigger an update everytime you change parameter x in the sketch, hence the model will be updated by coming out of the sketch. 

 

Please let me know if this makes any sense, otherwise, I will try to explain this with a more detailed example. 

 

Thanks.

 

Kind regards,

Mohamad Jenaban

Message 17 of 17
jakub.struszczyk
in reply to: -ianf-

This post should be marked as a solution.


@-ianf-wrote:

Figured out what our issue was here.

The parts that were exiting the sketches on edits had some ilogic rules in them containing;

 

InventorVb.DocumentUpdate()

 

This was running with a trigger;

 

Any model parameter change

 

The result was forcing the sketch to exit when editing the dimension.


 

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