Can Fusion create a true bolt circle?

[Anonymous]

Hello to all,

 I have looked for a solution in past messages seeking help with circular patterns. There are none that seem to relate to my issue. I have come from a shop floor environment where bolt circles are a common issue. I have tried the circular pattern guidelines. They work for machined pockets, plain circles, and center points. When I create a 3/8-16 threaded hole, using a .313" tap drill .75" deep, with threads .38" deep everything is fine. When I try to create five copies around a 5.0" dia. circle, the icon for creating a circular pattern is not darkened or capable of doing anything. In a post about two years ago, this did not seem to be a hot issue as far as the development group was concerned. Has this changed? 

 Can someone shed some light on either my inexperience with the product, or a way to do these features short of recreating each hole over at each point. My take from what I have read and observed, is that a circular pattern only works on two dimensional geometry.

Thank you and best regards,

Bob Queberg  

[davebYYPCU]

There are two circular patterns available, Sketch and Modelling, 

When using Create > Pattern > Circular Pattern you will need to select Features in the Dialogue Box, 

and select the hole and the thread when doing so..

Should work...

[etfrench]

You can do the circular pattern in the CAM workspace.  If you have trouble creating it, post here and I will make a screencast.

[dieselguy65]

something like this?

i am sure i didnt use your exact dimensions, i couldnt recall them once i was drawing. but it does work

[davebYYPCU]

Pattern in Model space as well.

[etfrench]

I'll go out on a limb here and guess that you're trying to select the 5" diameter circle when creating the pattern.  If this is true, then you may need to create an axis at the center of the 5" circle first, then use that in the pattern dialog. 

[Anonymous]

Hello ET,

 My procedure was to:

1) create a "drilled and tapped" hole @ X2.500 Y0.000

2) create a point @ X0.000 Y0.000 for rotation of the geometry

That was as far as it got. If the tapped hole was selected, the circle pattern was in a faint coloration.

One time, in desperation I selected the circle that described the hole diameter and it's center point. This gave me the original tapped hole, along with five other circles with center points nicely spaced.

 Please point out my errors, or ask any questions that are needed.

Best regards,

Bob Queberg

[dieselguy65]

I'm not sure, but i think if you look at what iuploaded, you can scroll
back thru thr timeline and see how i done it.
I'm out in thr field on s job now. But i have a bunch of work in fusion
this evening, I'll try to make a Screencast, and use your method.
This should do to get you thru. Best regards, Brian.

[etfrench]

There are three basic methods for creating circular patterns:

1. Sketch:

•     Draw a circle for the pattern.
•     Place a circle the size of the threaded hole on the circle for the first hole.
•     Open the Sketch Circular pattern dialog.
•     Select the hole circle for the Objects field.
•     Select either the center point or the perimeter of the pattern circle for the Center Point field.
•     Enter the number of holes.

2. 3d Model

  2A:

•       Using the sketch created in #1, select the Hole command for each of the hole circles.

  2B:

•     Create the first hole using the Hole command.
•     Create an axis at the center of the pattern.
•     Open the Circular Pattern dialog and select the face of the hole and the axis.

3. CAM

1.   You can just use the hole circles from the sketch.  Create the drilling and threading operations.
2.   You can use just the first hole circle from the sketch, then create a circular pattern of the drilling and the threading operations.
3.   You can do the same two methods with holes created in the 3d model.

p.s. I may need to learn how to count better

[HughesTooling]

@Anonymous if you're trying to pattern faces\bodies using a circular pattern from the create menu you need an axis to rotate around not a point.

Mark

[jasonhomrighaus]

Not sure where you stumbled but here is the process for you to observe hopefully that should help you figure it out.

[jasonhomrighaus · Accepted solution]

Take 2

[Anonymous]

Hello to all of the "Learned Ones",

 At last I have six 3/8-16 drilled and tapped holes spaced evenly around a circle. The spirit of co-operation on this forum is fantastic.  Again I thank everyone who shared their knowledge, and experiences so freely. 

 The abilities of Fusion continue to amaze me.

Best regards to all,

Bob Queberg