NX 9 Sketch Constraints

[enexuser]

Hello,

Is there any way to make the sketch constraints in NX 9 behave more like previous versions, i.e. selecting two or more items and having the list of available constraints change to whatever the available options are based on your selection? I'm finding that pre-selecting the type of constraint I want, and then the geometry, is more cumbersome. Is there a work-around for this?

Thanks

Ben

NX 9.0.0.19 Windows 8.1 64-bit

 

[JohnRBaker]

Starting in NX 8.5, you simply SKIP selecting the 'Geometric Constraints' function altogether.

Instead, without selecting any functions, simply start selecting the curves that you wish to constrain and you will see a 'shortcut' tookbar appear showing the valid constraints available based on the curves that you've selected so far.

Starting with NX 8.5 we changed the behavior of the explicit 'Geometric Constraints' dialog to work more like how constraints were assigned when using Ideas. This was done primarily for those former SDRC customers who have transitioned to NX but who still wanted to have an 'Action/Object' type workflow similar to how things worked in Ideas.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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Siemens PLM:
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[enexuser]

Thanks John!

That seems to work well with entities within the sketch; not so well constraining something in the sketch to a curve outside the sketch, from what I can tell. I tried constraining and endpoint of a sketch line to a line on a projected curve feature outside of it.

Ben

 

[JohnRBaker]

Yes, for selecting items outside the current sketch, you really need to use the 'Geometric Constraints' dialog but then those sorts of relationships can only be defined one-at-a-time anyway, so using the 'Action/Object' paradigm is not that much of an issue.

BTW, with NX 10.0, not only will you be able to select curves/edges outside the current active sketch, but if you're working in the context of an Assembly, you'll be able to select curve/edge references in Components other than the Work part with the option to automatically create associative WAVE links or not.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[enexuser]

Okay, thanks for the reply. Just making the leap from 7.5 to 9 and trying to learn the ribbon bar interface, etc. Mind open, learning new things.

Cheers,
Ben

 

[JohnRBaker]

Of course, this particular issue, Sketch constraints, is NOT a "ribbon bar interface" issue since the changes you're experiencing were first implemented in NX 8.5.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SDETERS]

Coming from the I-Deas world I liked being able to select the constraints type first then the objects. This way the constraints kind of filter for the objects that you can and cannot select. For example if select tangent first then you can select lines, circles and splines but you should not be able to select endpoint, centerpoints and or any other feature that you can not make tangent. So this was a nice enhacement in my opionon. But, with the above being said I am not totally against the way NX has these constraints set up in NX7.5.

 

[cowski]

Coming from the UG/NX world, it was a short learning curve and is now my preferred method for the same reasons given by SDETERS. I agree it was a nice enhancement.

www.nxjournaling.com

 

[carlharr]

Ditto cowski and SDETERS, the new method is MUCH better than the old method, faster, clearer and mainly it doesn't allow you to make "wrong selections" once you've chosen the constraint type, i.e. can't choose curves if you want co-incident, can't choose arc centres if you've selected equal rad etc.

A big improvement.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[SvenBom]

And what would be even nicer is, if one can predict, what will change after the constraint is applied. This is coming from a Solid Edge world.
For example:
1. draw two lines
2. select collinear constraint
3. select first line and then the second one. The second one will change its position.
4. now, undo the last constraint.
5. select collinear constraint again.
6. now select second line and then the first one. The change will be exactly the same as in step 3. Again, the second one will change its position.

When working in Solid Edge, the first line you select will change according to the second line. And this is the same for all the constraints. First geometry selected will change according to the second one.

And also, what the Geometric Constraints dialog box says in NX is this:
1. select object to constrain
2. select object to constrain to
I am not a navitve english speaker, so maybe I am wrong. But I understand those two lines as this. The first geometry, that I am selecting is going to change according to the second geometry, that I will select.

 

[JohnRBaker]

If you think that this is not working as expected or at least not how the dialog implies that it should be working, please contact GTAC and have them open an IR/PR.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.