Interpart linking in sketcher

[Ritchie]

Hello NX users,

Coming from Catia V5 I'm new to NX. I'm quite up to speed with NX already however there is something that continues to annoy and me. Probably because I don't know the rules, I have tried to get hold of these rules in both cast and NX help however without any luck so far.

The issue regards sketching in a part in an assembly. I would like to create constraints between this sketch and other parts in the assembly, for instance reference an edge of another part to create a distance constraint. I have found that sometimes I can select geometry of other components directly, and sometimes not.

A strange situation has just occured: When I'm creating new geometry in sketcher mode (for instance the rectangle command) I can directly select the edges of other components in the assembly. The selection scope is set to "Entire Assembly". When I try to constrain geometry to edges of other components in the same sketch (for instance "Horizontal Dimension") I can not select these edges. I have noticed the selection scope is limited to "Within Work Part Only" and "Within Active Sketch Only". This happens in the same sketch, straight after having created the rectangle. The only way to reference the edge for this horizontal dimension is to import the edge into the sketch via intersection curve or project curve.

I'm really puzzled as to why this is happening, can someone explain it to me?

 

[ChaseWichert]

If you are trying to create geometry it allows you to use points of the assembly components, but it is not associative. The only way to constrain or sketch associatively is to link the body, face, point, curve, etc. into the Assembly part. Catia did this automatically, depending on settings. In NX you have to purposefully wave link in the geometry that you want to constrain to or reference to.

NX 8.5.2.3

 

[JohnRBaker]

While it is true that when working in the context of an Assembly, you'll need to create 'WAVE-linked' geometry inside the sketch if you wish to create associative constraints that references the edges of the Components in the Assembly. However, that can be done automatically WHILE you're adding the Projected Curves to the sketch, which you must do anyway if you wish to create true constraints.

Below is a pciture of the dialog used to create the Projected Curves showing the required settings as well as the 'Create Interpart Link' icon that if it's toggled ON, as shown in the image, when you select the edges from the Component that you wish to poject into the sketch that these curves will be created ASSOCIATIVE to those edges automatically. If the the icon is NOT toggled ON, the projected curves will still be created, but they will be non-associative copies of the selected edges.

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.

 

[Ritchie]

OK thank you gentlemen, it's completely clear now. I'm familiar with working with WAVE link objects already so I shluld be fine. I just wasn't aware of the Create Interpart Link button.

But I guess this still means that when applying constraints I will have to include the referenced geometry manually (by using project curve for instance), whilst I can select the referenced geometry directly when I'm creating new geometry in the sketch? Just out of curiosity, is there a reason why or does this just happen to be this way?

 

[JohnRBaker]

The issue is NOT that you can't associatively reference geometry that has not been included, i.e 'projected', into the sketch, just that the geometry needs to at least be IN the part file in the first place.

Try this; open a new part and create a 'Block' using...

Insert -> Design Feature -> Block...

Now create a sketch on the top face of the Block. Now create a circle and as you drag it, place your cursor over an edge of the Block and you will see that the a tangent constraint is created. That's because the edge of the block is ALREADY in the same part file as the sketch. Now if the block had been a Component in an Assembly and you were creating the sketch in the Assembly you could still select the edge of the block (if you had the selection scope set to 'Entire Assembly') when you created the circle but since the edges are NOT actually in the Assembly file you couldn't create the constraint. Now if you had performed an explicit WAVE linking operation copying the edges of the Block into the Assembly BEFORE you created your sketch then you could create an associative constraint relative to the WAVE-linked copy WITHOUT having to first project it into the sketch. The only reason that we ALLOW you do that Project with an automatic WAVE link is to just provide one additional workflow that does NOT require that you do a bunch of WAVE linking BEFORE you start creating your sketches. This way the only links are those that you created as part of the sketches where they were really needed. It's just for the user's convenience, nothing else.

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.

 

[Ritchie]

Hi John,

Thanks for the elaborate answer. I have noticed now how the WAVE linked objects appear in the part navigator when I make a proper link to the referenced geometry. This will work for me!

Regards!

 

[SDETERS]

For reference There is a switch in the Cusomter defaults that lets this icon work. If you go to File --> Utilites --> assemblies --> Then Interpart Modeling tab. There is an option to turn this off and or on. If this is set to no this icon will still greyed out while you modeling.