Patterning in Sketch Mode

[bmichell]

What good is patterning in sketch mode when you can't use the copies to extrude in the model. I'm drawing a part that looks like a peace sign and need to remove the material between the spokes. I made one spoke and used the circular patterning tool in sketch mode to make the other two spokes. When I tried to cut the material between the spokes in the model, it would not allow me to pick the profiles. Did I do something wrong? Other people in my office also told me that they couldn't use a pattern in sketch mode to cut or extrude profiles.

[Ron Oldenbeuving]

What good is patterning in sketch mode when you can't use the copies to extrude in the model. I'm drawing a part that looks like a peace sign and need to remove the material between the spokes. I made one spoke and used the circular patterning tool in sketch mode to make the other two spokes. When I tried to cut the material between the spokes in the model, it would not allow me to pick the profiles. Did I do something wrong? Other people in my office also told me that they couldn't use a pattern in sketch mode to cut or extrude profiles.
bmichell (sorry, I dont know your real name), I created a quick part to try and emulate your problem, but found it worked ok (open attachment and drag End of Part marker to bottom). It sounds as if the sketch geometry you are working with may not contain fully closed profiles. Could I suggest you run sketch doctor to see if you have open or self-intersecting loops, overlapping curves or non-coincident endpoints. If all else fails, extrude 1 of your profiles, and pattern the resulting feature. HTH.

[bmichell]

Ron,

Thanks for your help. I had a number of open loops and when I closed them everything worked as expected. I now have to teach my engineer how to using patterning properly.

Brad Michell
Engineering Manager
Emco Wheaton Corp.
Canada

[jamesdill]

I am having the same problem drawing saw teeth in a sketch and am unable to extrude. Somone said i need to chain the teeth together? any ideas
Jim

[JD Mather]

It is almost always better to pattern a feature rather than a sketch.
Example do a pie-piece shape, extrude and then pattern feature.
If you must pattern a sketch then click the Red Cross when trying to extrude as a solid and run through the sketch doctor to repair the sketch. Patterned sketches often result in endpoints that won't combine without running the sketch doctor.

[robert.templeton]

When you draw your saw blade and tooth, I assume you sketch the base circle of the blade and then sketch one tooth, constraining each end of the profile to the base circle. That forms two closed profiles and each one can be extruded. When you create a pattern of the tooth profile, the ends of the tooth profile are on the base circle, but there is no coincident constraint to tell Inventor that the two entities are connected.

Here is a simple solution to the problem: close the tooth profile and create a pattern of the closed profiles. Draw a line or arc connecting the two ends of the tooth profile (a line between the two endpoints works nicely and is visible). Include that connecting line in the set of entities you pattern and each of the closed profiles can be extruded.

I also prefer to create patterns of my features instead of patterns in my sketches. I am more comfortable editing the feature pattern than I am editing a sketch pattern.