Instance feature along a path in NX 5. 1

[BOPdesigner]

Is there a way to instance a feature, say a hole, using a curve as a guide path? It appears that you can do this with geometry using the Instance Geometry tool, but I only see rectangular or circular array options for making a feature pattern.

 

[JohnRBaker]

That's correct.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Okay so you won't be able to instance along a spline, and I can see why certain complex cases are in fact beyond the scope of how the software is basically intended to be used.

It may not help you in this case but users have asked in the past for a solution that doesn't exist to a problem that can be solved with the existing tools. If the curve that you want to follow is straight for example then you just need to align your WCS with either the X or Y axis along the curve and then create an instanced array. Similarly if you're dealing with an arc you just have to define an axis to instance about.

Now if the feature that you want to instance is simple enough that you model it from the curves of a sketch, then assuming that you have to create instances along a spline, you can get most of what you probably want by locating a datum plane along the spline curve. You can define a datum plane along a spline and it is by default normal to that spline, and you can move the plane any distance you like along the spline by editing its parameters. So if you build a sketch of your feature based on the plane then as you move the plane then the sketch and therefore your feature model will follow. Having done all that you can then make copies of the model with the plane translated various distances along the spline, copy and paste ought to take care of that, but you may want to move your construction to different layers. At this stage the planes that the sketches will be built on will associate to separate curves, you may be able to correct that by editing their parameters to associate all with the same curve. At the end of the exercise I can add in a few expressions to vary the distance between the features, the only thing that I can easily manage is to vary the number of instanced features.

Best Regards

Hudson

 

[hudson888]

I worked an example based on your question and found that on re-reading the case may be even simpler, because you can position a hole center to a point and it is associative with that point. All you need now are points at intervals along your spline and you can start making holes. As far as I'm aware there is no way to make points along a curve associatively without doing some extra work. So you can construct planes at intervals along a spline as I described above, and then define associative points based on the intersection between plane and spline. In addition you'll have to create your holes one at a time, but the result has some useful parameters that weren't too hard come by.

Happy pseudo instancing

Regards

Hudson

 

[hudson888]

Correction in the last line of the second last post, the word "can" should be "cannot". Typo

 

[phillpd]

In the case of a hole and assuming you're using NX5.0.2.2.

When creating a hole, rather than using the Boolean option of SUBTRACT, change it to NONE. You can now use Geometry Instance and select the "holes" as the instance object.

Specialty Engineered Automation (SEA)

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a UGS Foundation Partner

 

[hudson888]

That sounds good Phil, but if you wanted to instance the object at equal distances along a spline what additional steps would you take to go about that task?

Regards

Hudson

 

[JohnRBaker]

Actually if holes are the ONLY feature that you're interested in, you can draw your curve along the face of the model and then place a point at one end. Then use Instance Geometry to create copies of the points along the curve. Once that is done, go into the Hole function and using the selection option of 'Point Set' select any one of the copies of the points that you instanced along the curve. You will now have a Hole for each point created. Also is you were to edit the number of points in the 'Point Set' the number of holes will update.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

John,

It sounds like this is a new method that takes all the hard work out of my earlier scheme of doing things. Is this new in NX-5? Another improvement that I'll have to try. Will there be some similar function for instancing other features? I could see how it might apply to bosses and pockets equally well, and that instancing features based on separate primitives is a challenge for the future.

Best Regards

Hudson

 

[velto]

BOPdesigner
If you have NX Shipdesign license you can use the tool non planar ventilation holes to do it with your own library holes (see the attached picture)
Velto

 

[BOPdesigner]

Thanks for your help. Johns suggestion works good for holes, Phils method works for other geometry, but you could have problems with orientation of the instanced geometry along the curve.

 

[JohnRBaker]

Yes, both the Instance Geometry (Points along a Curve) and Hole Sets (being able to select a single 'Point Set' as the origins of a Hole Set) are new for NX 5.0 (in the case of the Hole, NX 5.0.2.2).


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/