Instance feature along a path in NX 5.
Instance feature along a path in NX 5.
(OP)
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.





RE: Instance feature along a path in NX 5.
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/
RE: Instance feature along a path in NX 5.
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
RE: Instance feature along a path in NX 5.
Happy pseudo instancing
Regards
Hudson
RE: Instance feature along a path in NX 5.
RE: Instance feature along a path in NX 5.
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)
http://www.sea4ug.com
a UGS Foundation Partner
RE: Instance feature along a path in NX 5.
Regards
Hudson
RE: Instance feature along a path in NX 5.
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/
RE: Instance feature along a path in NX 5.
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
RE: Instance feature along a path in NX 5.
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
RE: Instance feature along a path in NX 5.
RE: Instance feature along a path in NX 5.
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/