Aligning to cylindrical parts 2

[Raddy13]

I'm working on a design concept that involves running a length through a metal cover, then bending it upwards 90 degrees and running it parallel to the cover. To help control vibration, I wanted to add a pin that will weld to the cover piece and the pipe. However, I cannot figure out how to align the pin to the center of the pipe. I have a "Touch" constraint to make sure the pin contacts the cover plate, but I don't know to make sure that the pin is centered on the yellow pipe shown in the picture. I've tried all the constraints and none of them seem to do the trick. I'd prefer not to do a "Distance" constraint, since the location of the pipe may move.

Unfortunately, the full model of the cover is marked as a secure component and I cannot upload the model. Any help would be greatly appreciated.

 

[Raddy13]

Another view

 

[JohnRBaker]

If the edges of end of the 'pipe' and the 'pin' are both circles you could try a 'Concentric' constraint but that will also force the two ends to be coplanar which may not be what you want.

BTW, what version of NX are you using?

John R. Baker, P.E.
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[JohnRBaker]

If you're running NX 7.5 or NX 8.0, I've attached an example which constrains a point at the end of the 'Pipe' to the axis of your 'Pin'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
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To an Engineer, the glass is twice as big as it needs to be.

 

[Raddy13]

Sorry, should have specified, I'm using 7.5. I actually got it to work by putting a distance constraint between the center axis of the pin and and the centerline of the vertical section of pipe, and setting the distance to zero, though I thought a "Distance" constraint of zero was the same as an "Align" constraint?

Anyway, thank you for your help, it is very much appreciated.

 

[mmauldin]

I would add a datum plane to the pin model that runs through the center axis of the pin, then align or mate that datum to the center of the pipe.

 

[jerry1423]

What I may do when constraining is change the reference set to "entire part", and use whatever datums are available, and then when done constraining I change the reference set back to what it was (Model).
The datums may not show, but the constraints will still be utilizing them.

 

[Raddy13]

Okay, I'm having a similar problem with another model (this one I can upload!). The spacers on the bracket are symmetrical, so the spacer circled in red should be at the same vertical height as the spacer circled in black. This time, my trick of using "Distance" between their centerlines and setting it to zero overconstrains it. I can't seem to add any datum planes to the assembly; I have to go to a work part to add points or planes, which then don't appear when I return to the assembly. If the parts had a flat top to them, I could align them at the same height, but I don't know how to do that with round parts. I also don't want to use a "Distance" constraint with the other spacer because if I change the position of one of the spacers, I want the other three to re-position automatically.

 

[cowski]

Add the datums to your component part file. I like to create a new reference set in the file, something like "ASSEMBLY_CONSTRAINT_GEO", and add the solid and mating datums to this reference set. Back in the assembly, change your component's reference set to the one that contains the datums, add your assembly constraints, then replace the reference set back to what you want to display in the assembly file.

You can simply change to the "entire part" reference set to reference the datums, but the display may be overly cluttered with other part geometry. I like the dedicated reference set because it makes the constraint geometry more obvious to others who need to work on the file and/or assembly (and a good reminder to myself a few weeks down the road!).

www.nxjournaling.com

 

[Raddy13]

Thank you so much for that, it worked perfectly. I've never used reference sets before, but that's certainly a handy tool to have. Thank you again!

 

[edgray]

I would use the Prefer Touch constraint, but under the touch constraint there are four orientation options. Choose the Infer Center axis option. This will keep the pin centered on the tube even if the tube moves or is rotated. The only problem is trying to find the constraint in the list later as it will be labeled Touch not center.

The logic of not having a constraint that is made for centering cylindrical objects escapes me but I am no fan of the new constraints system. I started using it as soon as I got NX5 in the hopes of learning what it does better that Mate but no joy.

This is currently my biggest beef with NX. The assembly system is not logical, clear, or user friendly. Which is a HUGE departure from the rest of the package. The only saving grace for me is that my assemblies are simple, if I made copiers or something I would be foaming.

 

[Raddy13]

Well, I can understand the difficulty with trying to align two 1-dimensional lines, because you need a planar reference to align against. It would be nice if the constraint dialog gave you a plane constructor sub-dialog or an option to select a reference plane (such as a nearby flat piece), but with the reference sets, you accomplish the same thing.

 

[JohnRBaker]

The issue with respect to having a "plane constructor sub-dialog" is that Assembly Constraints are being created in the CONTEXT of the Assembly and the Datums really should be created inside the detail Part files where they can be properly related to those aspects of the model that you wish to reference when creating the constraints in the Assembly.

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.