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pattern in assemblies

Pioneer
Pioneer

is there any way to pattern in assebly environment?suppose i have 6 bolts and washer i applied constraint between one set and now  i dont want to repeat same constraining procedure.is there any way to pattern constraints also?

6 REPLIES 6

Re: pattern in assemblies

Solution Partner Experimenter Solution Partner Experimenter
Solution Partner Experimenter
explore remember constraints option in assemblies.

Re: pattern in assemblies

Valued Contributor
Valued Contributor

If the bolt holes were put in using Pattern, or Array, you can use Create Component Array.

This will keep the pattern of the holes and the assembly constraints applied to the bolt.

 

Although in NX8.5.3, it is becoming more a hit or miss issue.

It will not consistently work, and I have to go back and manually add each part.

Re: pattern in assemblies

Phenom
Phenom

YES, It’s possible with NX what you are looking for.

I’m using it for a quite sometime now to automate my design process. I couldn’t find any valuable literature on this topic as most of the NX users aren’t aware of this kind of powerful functionality you find in other software. So I had to do a lot of research in NX, trials and errors to make it work. Unfortunately, most of the pioneer NX users haven’t seen out of the box methods to make their life easier and it’s hard to convince them to use new features.

Anyway, If you haven’t found a method yet, let me know, so I can take some time to compile the instructions going through my notes.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: pattern in assemblies

Phenom
Phenom

Over the weekend I typed the following:

 

This is what you have to do: (it’s very easy.)

  1. Use “Hole” command to create holes in the main block. Create a single sketch (internally or externally), to indicate the holes’ center points.
  2. Add component or subassembly.
  3. Create assembly constrains you want to have.
  4. It’s necessary to have a “Touch Align” constrain preferably with “Infer Center/Axis” to a hole @#1.
  5. Now click Assemblies ->“Pattern Components” and select the component; Pattern Def> Layout=Reference; <OK>
  6. You will see the components have followed the Sketch pattern @#1

 

Testing:

  1. Go to Constrain Navigator and examine the new constrains created.
  2. In the Name Column, RMB Select “Group by Components” and you will see the new Constrains created under each component.
  3. Delete the pattern you just crated.
  4. Check again the constrains; undo the last command (i.e.: delete) and you will see it’s automatically adding new components with respective constrains as you defined in the initial component.
  5. Go to #1 sketch and edit it to add/delete or modify sketch points and <OK>
  6. Examine the components, they must have had responded and updated following the sketch points. (sometimes I noticed NX hesitates to update immediately. Then must try by fully loading option or reopen the assembly.)

Since Sketch, Hole and Pattern Components are relatively new commands, most of the NX long timers don’t understand what their potential is. Trying to explain this is like signing to a deaf elephant. Smiley LOL

P.S. According to my previous experience, these new features still have a vast spectrum to develop further. I feel they are still rough and rigid.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: pattern in assemblies

Phenom
Phenom

Expected behaviour

(view in My Videos)
 

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: pattern in assemblies

Phenom
Phenom