Catia V5 Pattern 2

[atcoast]

I know in UG they have component array while in the assembly mode. How can I do a circular array of a part While im in the product and maintain mating constraints. (Im trying to create a bolt circle pattern in catia v5). Any help would be appreciated.

 

[atcoast]

Let me clarify what i am trying to do. I have an assembly of 2 circular flanges. One flange has 16 threaded holes in a circular pattern and the mating flange has 16 clearance holes in a circular pattern. Now I want to position one bolt into one of the holes using mating constraints. Then I would like to create a circular pattern of the bolt component to fill the other 15 hole locations and apply mating constaints automatically if posible. I am a long time UG/solidworks/catia V4 user and have been on catia V5 only for a few months, I find it easier in V5 to do things but then again I wish i had the UG and SW for other tasks, its a real give and take tug of war.

 

[kboy]

Ok, I trust you have the 3 parts within your assembly. The 2 flanges with the holes and 1 bolt.
The first key to this is to ensure that the 16 holes in at least one of your flanges was created using the circular pattern command as a part. Why you may ask...
Well in order to pattern the bolt from the assembly environment you have to REUSE the pattern which was used on the flange part.
Now select the bolt in the tree, click the REUSE pattern Icon and either hover the cursor over the pattern in the flange or pick from your expanded tree.
This will pattern the bolt with the same specifications as the flange.
The advantage is that you can switch on/off each one of the bolts individually.
You can play around with the settings within the REUSE functionality.

 

[kboy]

Sorry, I forgot your other request, you can position the bolt in a variety of ways.
To constrain use the coincidence command and pick the centreline of the bolt and bolt hole, or the surface will do. Then use the contact constraint and use the surface of the flange and the underside of the bolt head. Depending on your settings the assemblly may update in real time, if not you have to force an update, look for the black & white swirl Icon.
I use the functionality of the compass to get close then finally constrain, in other words drag the compass onto the bolt, Select the bolt in the tree to make active then press left mouse button and drag / rotating along the desired compass axis / plane, when close drag compass back into position using just left mouse drag, best to deselect bolt first.
My best advice if you are new is to obtain training, otherwise you will not unlock the true power or potential of Catia V5...

 

[atcoast]

Thanks, It was answered externally before i got it before i had a chance to repost. Yes i had the bolt positioned and just didnt know how to operate the "re-use pattern function. My mistake was i was trying to create a pattern inside the assembly to use, i didnt know I could re-use a previously created pattern from a detail part. Thanks anyway.

 

[jackk]

Great answer Kboy! I'm giving you a star for that.