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how to draw a gear???


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I try to do a pizze piece of a gear and then pattern it around...but if the gear teeth is some curve shape, it just always fail to do it...can someone please tell me how to do a gear???? in general term???
what steps are you using?

i generally use Pattern>Varying|Done. Select the dimension you want to pattern, then type in the increment angle. Then enter the number of teeth the gear has. I hope this helps....
gurveen.... he is using the student edition, so he won't be able to send it to you unless you have it too.
i need to know how to make a simple gear. i have used pro-e in the past , but for some reason to make a simple gear is just beyond me. basically i have a cut that i would like to replicate ever nth degree of revolution... and as such have tried to use the pattern abilioty of pro-e to no sucess..

i dont want to be mirroring my pattern a 100 times :)

You are probably constraining the sketch to a centerline with an angle dimension. When it rotates over 180 degrees it flips over and overlaps another tooth. To pattern gear teeth correctly make a datum at an angle, and constrain to it. Then pattern the datum and tooth together.
Put in a datum plane at angle first, model the tooth about that plane, then pattern the plane/group.

That is the trick.
One more suggestion won't hurt :). If you have the ability to create a surface transform, you can create your tooth using any references you desire.

Copy the surfaces of your tooth. Then create a surface transform that creates a copy of your copied surface (or it won't pattern) and rotate it by some angle about the coordinate system or axis at the center of your part. Pattern the transform for n-1 teeth to keep from overlapping your original tooth. Use a cut or patch feature to build your geometry and reference pattern it.

In general if your gears have a high number of teeth this will regenerate faster.
Having problems with overlappinggeometry on agear. Have done sofar:

1) copy surface of single tooth 2) surface transform of copy made in step 1, rotated 7.2 deg 3) pattern transformed surface with n-1 teeth with spacing of 7.2 deg . ( so far have created 1 solid tooth and 49 surface teeth that seem correctly spaced ) 4) patch the transformed surface in step 2, ( now have 2 solid teeth and 48 surface teeth ) 5) pattern the patch of the transformed surface in step 4, and get overlapping geometry.

Any ideas what is going on?
I remade the tooth constrained on a datum at a 45 degangle. Made a surface transform which did pattern, still would not work for solidify.I then changed the datum angle to 30 deg andCOULD solidify. Using the 45 deg angle, one of the pattered teeth aligned itself on one of the default datums ( front ). With the 30 deg angle, NO teeth are alignedon a default datum.

Could anyone explain what is going on?
Thanks for the Tip, Dell Boy.

I have been searching on the PTC site but could not find the gear tutorial, could you help me find it? Thanks.
One of the most common causes of patterns not doing what you expect is the constraints of the original profile. ProE has difficulties in "intelligently" easing constraints on the feature to allow it to pattern. Meaning that for instance vertical stays vertical and doesn't get rotated, alignment to datum planes is kept, ... Rotating patterns are an even greater challenge because of angles returning to their complement when going over 180


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