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# Patterning a Group (Rotational)

#### ptalk

##### New member
Can someone in here give me their expertise help on this subject? I have included 3 images. They all used the 60 deg. angle plane DTM1 (insert plane) as the Leader Dimension. I'm getting mixed results from different group features being pattern. Sorry about the poor image quality.

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My guess is that you've referenced some of the existing geometry when creating the first protrusion.

eg: if you have a dimension to the outer surface, this will probably fail when you try to go 360deg, since Pro/E makes circles in 2 halves. Once it gets past the join, the pattern will fail.

In the 2nd case, the datums are patterned at 120deg, but the protrusion must again have an additional reference (possibly a centreline in the sketch) - it goes on the wrong side of the datum, making it 60deg instead of 120.

Rotational patterns are still very untidy in Pro/E. My company designs almost entirely cylindrical parts, so we're very to dealing with them... but to start with there were a lot of niggles.

ttalk

The good thing is that, in proe there is seveal ways of patterning. If one way fail try a different. Sometimes in a rotation pattern, if you go -120 deg and two time works. Then modify it to -120 deg, 3 times because this is what you really wanted. This trick works for me, but it all depends on how I created the lug. Just my two cent ...

ptalk,

Features that have references to circular geometry won't pattern beyond the 180 degrees because ProE defines circles in two halves, as mentioned correctly by proed.

A robust method I use, especialy with a complex group of features to be patterned, is the following:

Create your detailed geometry which you wish to pattern with all the desired features as needed. Now create a surface by copying all the surfaces of the geometry to be patterned. Now transform this quilt by rotating it (no copy) around the central axis with the desired angle. Create a protrusion-use quilt to make it solid. Now pattern the transformed quilt around your part by clicking its rotated dimension. Ref pattern the protrusion- use quilt.

This method will speed up regeneration and you don't have to bother not to refer to circular geometry.

Good luck!

Huug

First things first, are your sketching refs correct ?

You should have selected a datum-plane or a face for sketching on and then DTM1 to be your left or right ref.

A side note on this:

As WildFire has done away with make-datums patterning like this now has to be done with groups in this manner. It was so much easier with make-datums as we only had to contend with a single feature.

Now we have to consider additional features and patterning groups to achieve the same goal.

What was PTC thinking ???

This is the way I create rotational pattern:

- create the first feature (or features)

- copy the features without dependency and give the increment as rotation (I prefer rotation about coordinate system). This results a group of features to be patterned,

- pattern the group created, you should have the needed angle available

- Finally you can delete the original feature (it does not affect the model, because the copy was created as independent)

The benefit of this procedure is that you can pattern more than one feature at time..

The most robust way I've found to pattern is to use make-datum to create a datum-plane to define the pattern dimension.

This way you only have to pattern one feature and not go thru the hassle of using groups.

This technique is good up to 2001 but as I believe Wildfire has done away with make-datum we may have to resort to grouping.

I'm at a disadvantage, I have no intention of going to Wildfire..

First of all, I would like to say thanks for all of you guys or gals help. Now, I have a better understanding of this command and solved my problems with the above models. One thing that I didn't quite get a handle on is the 2 halves of the circle, where does the half starts and ends? Does it start from DTM1 (angle plane), Front plane, or Right plane? Yes, I know I asked stupid questions but hey I new at this stuff. So, take it easy on me.....Just remember you were in me shoes once too .

When I have a problem with rotational patterns 'cause of the half arcs.

I simply create a centerline 90 deg to the one running through the center of my feature that has the angle dim on it, make sure there both going thru the center of the part the I mirror the geometry about the perpendicular centerline.

The key is to simply be at the start of the half arcs.

Just my 2c

Brian

if u have problem in these type of inbuilt rotational pattern go away with a simple procedure create a feature and copy move it with independent with the required center axis for required angle now pattern this copied feature.if u dont want the first one u can delete it

I had same problem too, but I did't stay too long to understand why this stuff happends. In that case, after I tryed several times to deal with this problem, I used copy/move/rotate option.

My experience has been copied, mirrored and patterned features can cause unexpected problems in the future. They are not easy to work with. Would it not be as easy to sketch the 3 features at the same time, utilizing copy/rotate in sketcher and constraints so only one feature was dimensioned?

If you're not on Misfire you can still use make-datum to avoid datum-plane cluster and having to use groups.

make datum is a very clean and robust way to setup your pattern variables...