How can I insert a point pattern from my skeleton in my part?

Question

I have used the technique from the answer video posted here https://community.ptc.com/t5/3D-Part-Assembly-Design/Is-there-an-easy-way-to-insert-fasteners-when-you-are-finished/m-p/816132 a lot when working with axis patterns where you have a lot of holes in a circle. I have used it with skeletons instead of multibodies though, because I do not have multibody functionality. So I would create a point in a sketch inside of the skeleton

and then create an axis pattern on it using the standard axis which is perpendicular to the sketch plane, so that the model tree of my skeleton and my assembly looks like this:

If I want to create different parts that use this pattern, I can create a new part within the assembly, leave it with arbitrary constraints, open it in a new window and create a copy geometry of the pattern leading point. Then I do a pattern, and it automatically creates a reference pattern. Next, I can create holes on top of the pattern leader and create a reference pattern as described in the video from tbraxton, so that my assembly and model tree for example look like this:

Because this technique worked very well for a radial pattern as I only have to make changes in the skeleton, I want to also use it for holes that have a different pattern. For example, I want to use holes in a point pattern. So, like I did in the previous example, I create a skeleton with the points. For simplicity, I only create a point which is dimensioned to the default axis, then create a mid line inside of the sketch and mirror the point around that midline, so that I have two points that are symmetric to the midline (I did the pattern inside of the sketch because I tried and it also does not work with the mirror feature outside of the sketch, because the mirror feature out of the sketch creates another element in the model tree which is not including the original feature so I can not use it for a reference.). So, my skeleton and model tree in this case look like this:

Next, I create a new part within that assembly, leave it with arbitrary constraints, open it and start with a copy geometry.

In that copy geometry, I select the first point I created. Now if I want to create a pattern, I have to go back to the assembly, and activate the part. I click on the pattern icon on top of the copy geometry I created first, but reference is greyed out

so I select point, select the sketch from the skeleton which I can only see in the assembly, and accept. But now, the points in the part relate to the location of the part in the assembly.

I would have expected them to represent the pattern that I also have in my skeleton. Does somebody maybe know how I can create a copy of the point pattern from my skeleton in the individual part, or what the proper way of how to do it is? (Like in the example of the radial pattern above.) Because I think I did something incorrectly. Thank you for reading and I would really appreciate a reply, it would make it easy for me to connect different parts with holes in corresponding locations.

tbraxton · Accepted Answer

Your idea is a good one and use of a skeleton for this will work but you will need to create the hole locations using something other than sketched points in a single feature in the skeleton. If you want to leverage the reference pattern through a copy geometry you can use any of the pattern tools and then pass the lead instance of the pattern through the copy geometry.

For a linear array shown in your example the two obvious patterns methods are a 2D dimensional pattern or a table pattern. to locate the hole centers. I would use 2D dimensional pattern for your example.

I have also used Creo notebooks (.lay files) to define the hole locations that are shared across multiple parts but that is a completely different top-down design tool and does not leverage reference pattern functionality.

As mentioned previously I would not mirror features as standard procedure. It is not wrong per se but as I mentioned the behavior of mirrored features is more trouble than using a different method in most cases if your models are modified after the mirror.

Mirror within sketcher is fine and I use this often, but it is not a "pattern" data structure within the Creo environment.

tbraxton · Answer

The problem is with the point "pattern" you have created in the skeleton model using the mirror within the sketch. When you sketch points, this is not a pattern in Creo it is a sketch feature. As you know this can be referenced for patterning but the reference type when doing this is sketch. When you pass this point through a copy geometry feature it is not a pattern or a sketch in the derivative part and therefore cannot be used as a pattern reference.

To implement the design intent that you are attempting, create a pattern feature in the skeleton model and then copy the lead instance of the pattern as you have done with the axial pattern, and it should then work.

Creo 7 example models are posted for review.

In the skeleton model do the following:

1) Create a datum point feature in the skeleton model

2) Pattern this point as required

The skeleton model tree:

In the derivative part

1) Copy the lead instance from the skeleton model point pattern

2) Pattern the lead instance using reference pattern

The model tree of the derivative part:

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