Circular Pattern Command Problem

[vertical horizons]

I created a circular plate, and extruded a hole through it at an 18° angle.

 

When I attempt to use the "Circular Pattern" command, I have a problem.

 

For "Pattern Individual Features", I can select the extruded hole. But, when I want to select the outer edge of the circular plate for my axis, the edge will not highlight.

 

How can I select the edge? What am I doing wrong?

 

I have enclosed the .zip file of the .IPT.

Hole Problem.zip

[JD Mather]

Works here just fine (on your part).

Are you changing the selection tool to select the Axis in the Circular Pattern dialog box?

 

You should be selecting the cylindrical face (or the z axis in the browser) not the circular edge to define the axis of revolution (I would use the z axis - the BORN Technique).

 

Also, I noticed that Sketch 1 & 2 are not fully constrained - I thought we covered this ground?

 

And, you have a grounded workplane - not good practice. You should have a sketch angled line used to create that workplane - much easier to edit if needed.

 

Would you like for me to walk you through this step-by-step or do you want to figure this one out on your own?

[vertical horizons]

...Would you like for me to walk you through this step-by-step or do you want to figure this one out on your own?

 

Give me a little while to mess with it to try to figure it out.

[vertical horizons]

...You should be selecting the cylindrical face (or the z axis in the browser) not the circular edge to define the axis of revolution (I would use the z axis - the BORN Technique)...

 

That was my problem. I was choosing the circular edge, instead of selecting the proper axis.

 

...Also, I noticed that Sketch 1 & 2 are not fully constrained...

 

Yes. You are right. I did not constrain them. That's one of those things that I will have to keep reminding myself to do, until it becomes second nature.

[JD Mather]

If I were doing the model here is how I might do it:

Three sketches

Your first sketch changed to delete unconstrained circle and add vertical construction line to hole position.

Second sketch on YZ plane to define extrusion height and hole angle.

Workplane on endpoint of angled line.

Sketch3 on new workplane for hole diameter.

 

Extrude large circle and select .75 dimension from Sketch2.

Extrude small circle Cut Through All Mid-Plane.

 

The part could be simplified even more with only one sketch.

A rectangle to revolve the disk and an angled rectangel to revolve cut the hole.

[JD Mather]

Here is the simplified method all dimensions in one sketch.

Revolve the disk.

Revolve - Cut the hole.

Circular Pattern the hole.

Done.

 

No extra workplanes created.

No extra sketches created.