How do I put a multiple holes in a circular pattern on a cylinder

cedric_orejola

I am struggling with adding multiple holes around the outside of a cylinder. The circular pattern only lets you work on the plane you are sketching. Is there a way to have a hole applied to the outside but using the circular pattern on a plane normal to the circle?

shanshan

cedric_orejola,there are two kinds of pattern in Onshape, one is in the sketch as you metioned , the other one is the feature list include face pattern and part pattern,please see the below video ,hope  it is helpful to you!

cedric_orejola

shanshan  That was very helpful! thanks a lot

daniel_chow

shanshan said:

cedric_orejola,there are two kinds of pattern in Onshape, one is in the sketch as you metioned , the other one is the feature list include face pattern and part pattern,please see the below video ,hope  it is helpful to you!

May I ask what program or app you used to create that animated GIF?

Couldn't you save a few steps by making a blind hole with the hole tool then using the circular pattern tool?


Also wanted to mention for anyone else searching out how to do this, the circular tool is not located in dropdown menu as part of the pattern tool. 

brucebartlett

@daniel_chow

For Gif recorders see https://forum.onshape.com/discussion/comment/13813#Comment_13813


I haven't tried but I would have done the same as @shanshan because unless it changed recently the pattern tool doesn't accept features. 

shanshan

daniel_chow， I like using “LICEcap” for recording video which format is GIF, it is very convenient, you can try !

daniel_chow

Link to public document

Does anyone know how to use the hole tool to make a circular pattern around a spherical object? I can do this using the method posted by shan in the above post. But I've been trying to use the hole tool to create a circular pattern: 

shanshan

daniel_chow, please click "face pattern" in the dialog box of "Circular pattern", and choose all the faces of the hole in "entities to pattern"!in your model ,the hole depth is too big ,that's why you could not pattern the hole, please check it !

daniel_chow

Thank you Shan it worked!

And for anyone else searching up how to do this, be sure to check out this onShape tutorial on making a pipe flange
https://www.onshape.com/cad-blog/lets-make-a-pipe-flange

You'll use the revolve feature to draw a round object, then use the circular pattern tool to patter a hole around the flat surface of the flange. This tutorial will only take < 10 min drawing the model from scratch. It offers a third way of using the pattern tool different from the two method discussed above. 

jakeramsley

One trick you can do when doing a face pattern of holes is to use the "Create selection..." tool on the context menu.  With the hole option selected, the system tries to infer the hole based on a single face selected.  This way you should be able to get all faces of the hole.

1. Right click on the canvas and choose 'Create selection...'


2. In the 'Create selection' tool, click the drop down and choose 'Hole'.  This will try to infer a hole based on the faces selected.


3. Select one of the faces of the hole.  Notice that the rest of the faces should highlight as well.


4.  Click 'Add selection'.  Notice that your one selection has now put in four selections in the circular pattern dialog.

shanshan

jakeramsley I have not noticed "creat selection" until you mentioned it, thanks for sharing , it is more convenient!

daniel_chow

Yes, thank you, will try later tonight!