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Copy/paste group of holes


Copy/paste group of holes

I am designing this radial engine (see image), and have to put in the holes for the cylinder heads all around the crankcase. As you can see I have put in 8 of the holes, but I have to repeat this process 4 more times for a total of 40 holes. Is there an easy way to copy the holes in groups and move them to the other faces? For example take the group of 6 on the left face, and copy them as one unit. Thanks


if this is what you are looking for, then group the holes and use the pattern option.


You can pattern holes about an axis. You sometimes have to group features to make sure the pattern option is available for multiple features. Sometimes pattern can be a bit touchy but you will get the hang of it.

Good patterning habits will also help you when it comes to assemblies. Patterned holes can drive patterned assembly parts such as fasteners.

This might give you an idea of how these were grouped and patterned: This is Creo/Pro 2.0


Center large hole grouped with patterned bolt circle (5x)

Linear patterned side holes (2x)

Grouped holes from both faces

Patterned group (6x)


Have u tryed to do a copy / past special ? This would be the thing that prefer because patterns of patterns never a good idea since u can have to change some things in midle and that will be a problem.

Hugo Barosa

Wow, thanks guys, this pattern feature is really neat! It worked excellently.

Of note, you can create a group and pattern it as mentioned, or you can "reference" pattern the smaller holes to the large hole. This allows a little greater flexibility.

Good point, Frank. I am not sure which method is more stable in the long run.

Glad we could help, Aaron!

I think the reference pattern gives more flexibility, as if you have a group of 5 things to pattern, you can delete one of the middle ones an not have an issue, whereas you'd have to delete the patterened group, then ungroup, delete the feature, then regroup, then re-pattern.

Of note, I've had some instances where a patterened group wouldn't work, so I HAD to reference pattern some features, but have also has the reverse case happen. In my album posted here, I modeled a prototype Coke bottle with a handle, and had that exact issue trying to pattern the grooves. THAT was a fun model......especially having to tweak it to get it to shell as thin (.010 I think) as I did.

But, I wonder if you could actually cheat and select all the instances of a feature in a patterned group and have them not regenerate. Hmmmmmm.......

Indeed Frank. Reference patterns fail more often than not. they are very particular as to what the original pattern feature was tied to. This is what I get when I removed all the groups:


And the pair of holes on top are not related in any way to the original pattern so the reference pattern option is not available.

Although the points about sustaining groups is acknowledged. You cannnot move the insertion point nor can you just change things on the fly and expect the groups and patterns to change. It seems more a bandaide to allow simplified trees and patterning multiple features.

In this case, I think that using relations in the patterning dialog for each set of features is more consistent.

edit: I have been trying to add a relation for the number of instances with relations and it is failing miserably. The number of instances for a pattern is a "pNN" numeric value. For some reason, it accepts it in relations but it remain the value you initially entered -in some cases!-. I think the Creo interface made using relations just that much more difficult. I will have to test this further. I have the yellow stop light on and no issues are being reported. This is frustrating!

I had to quit the part and start over. I added the relation to the feature rather than the part and it is working now.

The array was set to 5 and the angle was set to 60. You can enter the variable in the angle dimension when creating the pattern, but I haven't found a way to add the number of instances as a relation variable in the initial dialog or in the "edit" dialog after the fact. I had to enter the relations dialog after the fact to apply the variable. Seems very cumbersome.

No more groups and the top level patterns are related to "array" and "angle" They were all driven from the axis.

Of course, you also have the number of instances with a specified angle in the pattern dialog. An often overlooked choice (the little angle icon).


I wouldn't say they fail more often than not, but you must be very careful how you set up the initial references, and then the references of the referenced patterns to the initial pattern. Most times it is as mentioned simply easier to pattern a group, but sometimes that fails and you have to do the reference pattern. dunno why, but it's like all those other glitches. You just need to explore all the Pro/WORKAROUNDS.....

On the relations thing, sounds like a regeneration issue.

I rarely use relation for anything but populating drawing formats. This exercise showed me the importance of using feature based relations as opposed to part level. Never worried about that in the past. In this case, it caused havoc. I still have a lot to learn about relations and parameters.

I do a lot of work with radial patterning and getting screws to assemble easily using reference patterns is quite important to me. Having patterns fail is a real problem with me. Reference patterns on radial trajectories have been particularly troubling. Funny thing is, the little black dot preview shows it properly, but that is not what it ended up doing.

Patterns in general can be tricky. You have to make sure the initial references don't get FUBAR'd, particularly on revolved patterns. I think this is a glitch buried deep in the code, that's been there for years. Pro/E splits cylinders in half, and I've found a LOT of things fail right at that bisecting line. Remember, depending on your settings, a negative number simply flips things. I've found, for a truly stable pattern or geometry (such as for instances where you truly want a negative rotation) rotated about a centerline, don't use a datum plane thru an axis related to, say, the front datum. Instead, use a point related to a coord system rotated the correct angle, then us a plane thru the axis and point. That way 5deg is always 5 deg, and -5deg is always -5deg. Try that if you're having issues.

Just to make sure I have the order straight.

1: Make a coord system on your centerline.

2: Make point at angle defined by created coord system.

3: Make plane through coordinate system axis and point.

And this stops angular features and patterns from occasionally reversing direction for no discernable reason?

If this works, bless you sir, you are a saint. A crotchety, cantankerous saint, but a saint nonetheless.

22-Sapphire I

Yes, on all get off my lawn!

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