Remember constrain in NX for part family parts. 1

[ashivu123]

Hi I have come across the option Remember constrain in NX function of this is whenever your adding component to the assembly it will ask you select the surfaces FROM to TO which surface component to be assembled.

In similar method I like add this user interface to the part family members I.e. hardware’s. Does anybody how this can be applied to the part family members? So that when end user adding the hardware to the assembly it should ask him to select the surface.

 

[SvenBom]

1. create a master file for Part Family. No member parts created yet.
2. place this master file in the assembly with appropriate constraints
3. use Remeber Assembly Constraints for this master file
You can close now this temporary assembly. It was used just to create those constraints.

Open this master file and create Part Family. You can also generate each member as separate part file, if you like. If you do this, each created member will also have the RemeberConstraints definition.
When the Part Family is created, open new assembly:
1. place master file in the assembly.
2. select appropriate meber
3. now, you don't have to select the assembly constraints and faces on the part family model. You just have to select the target faces.
4. and if you place the member, that was generated as a separate part, it will also be positioned with those remembered constraints.

Regards.

 

[JohnRBaker]

One thing that SvenBOM may have overlooked and that is that in his first workflow, remember that you have to actually SAVE the Part Family template file after the Assembly constraints were added and remembered. The temporary Assembly can be tossed without saving it, but the master template MUST be saved somewhere along the line.

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.

 

[ashivu123]

Thanks SvenBOm and John,

Touch Constrain for two mate two surface and Align for to align two circular faces.
When I called the template part or child part in to the assembly touch face is highlighting and when I select the align its not highlighting surface. Even after selecting target face to align the part is not positioning correctly as like in assembly constrain save condition.

 

[JohnRBaker]

On something like a washer (or anything circular) where you could line up two concentric circular edges I would opt for a simple 'Concentric' constraint. And if I were creating these parts using NX 9.0 I might even consider using the new 'Align/Lock' constraint, which in this situation would be similar to using a 'Concentric' constraint only the result would leave NO degrees-of-freedom whatsoever.

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.

 

[ashivu123]

Hi john, I tried with ‘Concentric’ constraint and it is working fine. It is highlighting circular edge initially I was interested in selecting surface rather than edge. Thanks

 

[Alfonz]

Is there anyway to use remember contstraints if you have already created the part families individual parts. I just tried that and though remember constraints works on the template, it didn't populated that out to the family members.

Thanks.

On NX 8.5

 

[JohnRBaker]

When you open a Part Family Template and while in the Spreadsheet, there is an option under the 'Add-Ins' tab to 'Update Parts' which will replace the previously created family members with new updated copies.

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.

 

[ashivu123]

Yes you can do that for already created family members.
1. Apply remember constrain to the template part.
2. Verify template part constrains (if required)
3. Save template part.
4. Go to spread sheet select rows of all the family members
5. In add ins tab slectupdate parts and save family

Now you get that options for family mebers too

 

[Alfonz]

That did the trick, thanks guys!

Al

 

[Toost]

Another nice extra is that IF you rename the constraints BEFORE you run the "Remember constraints" , the new names will be the prompts when adding the component. i.e "align" renamed to "centerline", "touch" renamed to "touch_head" or similar logical names.

Regards,
Tomas

 

[Alfonz]

Great idea Tomas, thanks!

 

[KhimaniMohiki]

You might want to also consider applying 'product interface' to restrict users selection to certain faces. Take a washer for example, you can restrict the faces available for assembly constarints to just the inner cylindrical face and the flat mating face.

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[JohnRBaker]

Also, if you give consistent names to the mating faces/edges for all of your similar families, such as the different Nuts, Bolts, Washers etc, then you can do a Replace Component and even if the parts come from totally different Part Families, the Assembly Constraints will automatically be reassigned correctly. For example, if the mating faces/edges of the master templates for a Hex-Head Cap Screw and a Socket-Head Cap Screw were given the same exact names, even something as simple as 'Face1' and 'Face2' or 'Edge1' and 'Edge2', this would be sufficient for the system to automatically reassign the Assembly Constraints when doing a Replace Component, even if the parts are coming from different Part Families. Just make sure that in the 'Settings' section of the 'Replace Component' dialog that the 'Maintain Relationships' option is toggled ON.

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.

 

[ashivu123]

Hi John,

I got a new situation that i have to apply remeber constrain to the pin. Pin will protrude some distance in the assembly. I selected "Distance and Concentric" constrainss to remember. After adding to the assembly constrains were fail due to pin will not protrude outside. Since I have applied concetric pin is not protruding. Is there any other way to make pin is concenric to hole??

 

[JohnRBaker]

You can use 'Touch Align' with the Orientation method of 'Align' or 'Infer Center/Axis' to align any sort of cylindrical pin/shaft to a hole.

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.

 

[ashivu123]

Yes I used 'Touch Align' with the Orientation method of 'Align' or 'Infer Center/Axis' to align. However while adding componen to the assembly it will not highlight align face or axis in the component.