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Circular pattern with rotated instances?

Valued Contributor
Valued Contributor

I'm trying to create a circular pattern where the instances are sequentially rotated 180° about their radial centerline.  I thought maybe this could be done using a "CSYS to CSYS" orientation.  So I tried it, with the "Specify From CSYS" kept at its default, and the "Specify To CSYS" rotated 60° about the Z-axis and 180º about the Y-axis (which is aligned with the radial direction of the part).  Below is what I got (highlighted part is the original).  As you can see, the first instance is in the correct orientation, but the remaining are not.  When properly aligned, the ends of each instance should touch, forming one continuous "wave".  So apparently there's something I'm not quite understanding with how this works.  Any thoughts?  Thanks!

 

pattern_rotate.png

 

 

6 REPLIES

Re: Circular pattern with rotated instances?

Siemens Genius Siemens Genius
Siemens Genius

You could 'adjust' your input so that it is a complete 'unit' for the pattern?2017-03-14 18_18_04-NX 11.0.0.33 - Modeling - [model11.prt (Modified) ].png

 

 

Re: Circular pattern with rotated instances?

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

Or use Orientation: Follow Pattern, and then clock every other instance (Hint: each instance in the graphics display has a tan square handle, right click the handle and choose clock).  Here you can see I've clocked two instances, selecting "User Defined" on the Clock dialog:

Screenshot - 3_14_2017 , 12_08_25 PM.png

 

 

Re: Circular pattern with rotated instances?

Valued Contributor
Valued Contributor

Thanks for the responses!

 

I could mirror the original (to create a symmetric part) and then do a normal circular pattern.  But I was curious if I could do this with the pattern command alone.

 

I wasn't aware of the "clocking" feature.  The problem with that is I need this to be automated.  The number of instances will eventually be controlled by an expression, so I need it to update automatically if that parameter changes.

 

Using a CSYS to CSYS orientation seemed promising, but for that to work the CSYS needs to rotate with the instances as they are created (so the CSYS axis flipping the part 180° is always correctly aligned).  The pattern command seems very powerful, so I wouldn't be surprised if it can do that.  It's just not clear how.  Too bad the documentation doesn't provide more detail on this.  

Re: Circular pattern with rotated instances?

Phenom
Phenom
  1. Open the “mf_pattern_asm_20170315.prt”* file
  2. In the Assembly Navigator> Unpack All
  3. Select the first  component in the list “mf_pattern_20170315.prt”> Make Work Part
  4. Go to expressions or double click the body and change “ANGLE” to15;20;30; 45;60 or 90.
  5. You may notice the assembly is automatically updating as your design intent.

When you are mirroring component, make sure to make it assossiative:

mf_pattern_20170315.JPGmf_pattern_02_20170315.JPG

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Circular pattern with rotated instances?

Valued Contributor
Valued Contributor

Michael,  Thanks for taking the time to put this together.  I looked through it and learned a few things (like the extrusion with symmetric offset; didn't realize you could do that!).  One thing I didn't make clear in my post is this is intended to be one component (not an assembly).  But I could do something similar by mirroring the "Z" extrusion and patterning that.  

 

What prompted my post though was an example model I saw of a chain, in which a feature pattern was used (via a CSYS to CSYS orientation) to offset and rotate each link by 90°.  Very slick!  It made me wonder if something similar could be done in a circular pattern.   I looked into it a little, but couldn't get it to work.  I may revisit it later, but doing a mirror is pretty simple.  So it would mainly be a learning exercise.

 

Thanks again!

Pat

Re: Circular pattern with rotated instances?

Phenom
Phenom

You are welcome!

It’s much easier to automate multibody component. checkout the added part and just chenge the ANGLE.

Another point I would like to highlight is in a sketch; you could make curves or points symmetrical about a plane or a line (construction). Most NX users drive this symmetricity with an additional expression (=ANGLE/2)

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW