[Creo 7.0] Assembly mode - Can I pattern same parts in diferent directions?

[cadbart]

Hi,

For a long time I've thought about using Pattern feature for different directions. Let's say I'm in assembly mode, I've got a simple steel structure with many connector just exactly as below:



Now that's ridiculous to insert every single element (connector) separately part by part. So we can use the Pattern inside assembly mode of course. So we need to (or maybe not) use 4 Patterns because connectors are placed in different dircetions like in the following picture:



I'd like to use only one Pattern for this operation but still keep directionality of these connectors. When I pattern all connectors with one Pattern I'm unfortunately losing this directionality as follows:

 
Therefore I've got a few questions. 

1. Is it even possible to achieve that - using one Pattern and ain't losing the directionality?
2. If the 1 point is impossible, what is the good practice for this example (and similar)? Should I create 4 Patterns separately?
3. Is the good practice to use Patterns in assembly at all? Using it also has the downsides e.g. we cannot restructure parts/assms which are patterned (e.g cannot move existing Pattern to another assembly).

Thank you in advance for each reply!

[pausob · Accepted solution]

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Your questions make me think of the bigger question to ask - how is this CAD model is intended to mimic the real life assembly of the part?

It seems you could do your whole GATE.ASM with 2 sub-assemblies, and each would have 1 pattern of connectors.... in this very symmetric example.

But is this how you would actually put this together?  Your assembly structure implies that the tubing is welded into a picture frame and then the connectors are laid out on top of it and welded to it.  In this case, it absolutely makes sense to pattern the connectors inside the assembly.  You can make a layout sketch in your top level assembly which will contain coordinate systems that specify the location and orientation of the connectors.  Then assemble the connector part via coincident coordinate system constraint to one those sketched coordinate systems, and then use the so called "point pattern" - see attached link to a youtube demo video.

One thing not mentioned in the video is that it's a good idea to always specify the origin of the 1st instance - search "alternate origin in sketch patterns" discussions about this esoteric point.

If the alternate origin option is not used:

[cadbart]

Wow, thank you @pausob, your reply is dope! Till today I've always thought about inside-sketching CSYS and CSYS constraint as useless features. I didn't know these are so powerful.

That approach is great for small numbers of patterned parts but what if we've got 40, 60 or even more patterned stuff? Setting 60 CSYS inside sketcher by hand is hugely monotonous and annoying especially since we don't have any pattern feature inside sketcher in Creo. So what about this type od design case?

Sorry, but I cannot see any "alternate origin in sketch patterns" topic on this forum and Google.

[pausob]

Seems that the wording "alternate origin in point patterns" will yield more results.

https://community.ptc.com/t5/3D-Part-Assembly-Design/pattern-error/m-p/636605

For in-depth understanding of the alternate origin issue, I found this article / video:

https://community.ptc.com/t5/Creo-Parametric-Tips/Understanding-patterning-of-a-standard-hole-with-point-patterns/m-p/440311

Yes, the sketched point pattern only works well for small number of instances.  Another limitation is that it's a 2D sketch...

If you need to manage 60 of something, then I think that you should look into using table-driven patterns.

Table-pattern your coordinate system:

Then assemble your connector to the 1st instance.  Then pattern-by-reference the rest of the connectors:

That way you can manage and display the design intent information in tabular form...  Also, these tables are manipulated via MS-Excel, which makes generating 100's of instances fairly simple:

[cadbart]

@pausob thanks again for your reply! Speaking of alternate origin this option is automatically and correctly marked when using Point Pattern in Creo 7.0 (and doesn't placed inside Option tab - just on top of the ribbon next to field of choosing the sketch of the points). So Creo's improved itself in this matter over the years 😉

When it comes to the Table Pattern I actually use it sometimes but didn't know I can work with MS Excel directly to maintain the Table (which in Creo is a little bit annoying if you ask me). But when I asked about patterning many stuff e.g. 60 parts I thought about the connectors placed like in the question's picture. Your example contains the parts patterned like stair-shape but what about the patterning many of the same elements (e.g. 60 or 80 connectors) with different direction? Can we make it easily by only one Pattern? 

[pausob]

Glad to hear that the alternate origin pattern issue has been fixed by PTC.  I'm still using Creo 4, so I wasn't aware of that development.

I forgot that to use Excel for the editor of tables, there needs to be a configuration option

part_table_editor excel

in your config.pro

If you examine the screenshots in my example, note that the dimensions being controlled by the table are the x,y, z coordinates and also angle of rotation about the Z-axis.  In this way, you can use table patterns to locate and orient all your connectors in one pattern.

I will say having patterns within a sketch would be useful - especially for those more comfortable with designing using visual means.  Then again, tables can be generated automagically - if you can use excel and its calculation and programming powers.  Also, instead of showing 100's of dimensions on the drawing, you can get the table "for free" to provide the list of coordinates to the downstream manufacturing processes.

One thing that would be nice if the pattern table data could be displayed on a Creo drawing.  I wonder if someone knows how to do this.

[cadbart]

@pausob OK, everything is clear 🙂 Again, thank you very much for your help!