Circular Pattern error

[damlars09]

I am trying to create a circular pattern that will create "teeth" on the upper face to help align parts with in a known angle rotation change once created. Everything goes well, and pattern shows up as intended on preview generation but once created it misses sections of the pattern. I have tried the other compute options but to no avail. As well as using faces vs features. Any insight as to what could be causing this would really help me on deepening my CAD problem solving skills. File should be attached for anyone's curiosity 

[etfrench]

Instead of creating the tooth form by an Extrude/Cut operation, create it as a new Component or Body. Use that to create the pattern, then Combine/Cut to create the teeth.

What did you select for the axis in your circular pattern?  I created a new axis by extruding the face, then created an Axis through Cylinder.

[damlars09]

I used the outside edge of the pipe as my axis. 

I am unsure how I can make that shape a body or component on its own and maintain the shape I want. I used the split face tool and then a push/pull command so it will have a taper that goes towards the center. When ever I do it in a way that I know I can create a separate body from , i.e extrude command, it doesn't have that taper on the sides. Even then I tried to create a circular pattern with that body ,albeit not the correct shape I want, and it worked but then when I tried to combine/cut it gave me an error of unable to Boolean bodies.

[jeff_strater]

@damlars09 - I took a look at this today.  This is a bug in Fusion.  To be honest, I've never tried to pattern a Split Face + Offset Faces before.  Knowing a bit about how pattern works, it's not too surprising that this fails, but the way it fails is very strange...  I created FUS-61403 for this bug.

I played with a couple of options, and finally got something to work.  Take a look at this screencast (with audio) to see what I did - it's not a great workaround, but I think I end up with the geometry you need.

[laughingcreek · Accepted solution]

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@damlars09 wrote:

I am unsure how I can make that shape a body or component on its own and maintain the shape I want. I used the split face tool and then a push/pull command so it will have a taper that goes towards the center

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the face that your push/pulling isn't going to give you that even taper all the way around the object because the surface curvature varies as it goes around.

The extrude that @jeff_strater  is good if that is the geometry your after. the "hills " and "valleys" converge toward the center, but the hills tops also slant down.  this is the way it needs to be if you want to mill the grooves with a cutter.

if you want the hill tops to be flat accross the top, you can loft it like in the attached file.  note that this creates twisted planes, but is the same as what you would expect if you pushed, pulled on a cylinder. 

you can also loft the profile to a point at the center, which will give you a flat hills, but valleys that slant upward.  doing like this will get you back to having flat planner faces that could be milled.

[damlars09]

Thank you for the workaround! I was able to get these same results before you posted this but the only thing I didn't like about it was that the "tooth" profile would cut into itself and end up lowering where that top point sat. In my head this would throw off the angles of the pieces when two would be put on top of each other (each piece of pipe is at 15 degrees to use 6 to make 90 degrees in total). I don't know if that small change would make a larger more drastic change once you compound it with more pieces. 

[damlars09]

This looks like exactly what I am trying to accomplish. I will try this method on the bottom and print a couple out see if it works as intended. Thank you very much! There is a very steep learning curve with CAD if you don't have any mentors to bounce ideas off of.

[g-andresen]

Hi,

Here is a short documentation with reference to the neuralgic point:

günther