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Making 3 radial holes in a cylinder
hansrudolf
Member Posts: 57 ✭✭
Hi all,
I could have worded my question in many different ways, but I think that above is the easiest to understand.
I have drawn a simple cylindrical form,and want to place 3 radial holes with 120 deg. angular distances around that cylinder.What I could do was making a new plane, parallel to the top plane and with offset = radius of my cylinder. On this I could place the first of my 3 holes, all ok until now. But I found no way I could define the two other planes, which are parallel to nothing. I tried to add a triangular extension to the cylinder, so I had 3 faces on which I could define new planes, and could draw the other holes. But when I delete the triangular extrusion, the holes disappear also...
I'm sure for such an easy problem there must also be an easy solution?
Thankful for any help,
Hansrudolf
I could have worded my question in many different ways, but I think that above is the easiest to understand.
I have drawn a simple cylindrical form,and want to place 3 radial holes with 120 deg. angular distances around that cylinder.What I could do was making a new plane, parallel to the top plane and with offset = radius of my cylinder. On this I could place the first of my 3 holes, all ok until now. But I found no way I could define the two other planes, which are parallel to nothing. I tried to add a triangular extension to the cylinder, so I had 3 faces on which I could define new planes, and could draw the other holes. But when I delete the triangular extrusion, the holes disappear also...
I'm sure for such an easy problem there must also be an easy solution?
Thankful for any help,
Hansrudolf
0
Best Answer
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@hansrudolf - you need to change the first option in the Pattern feature - it defaults to Part Pattern - change it to Feature Pattern. For planes like "tangent to cylinder", you will need to create some construction geometry first. A better option for creating these types of holes is coming soon.Senior Director, Technical Services, EMEA6
Answers
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Hi.I'd make one hole and then use the circular pattern tool to add the 2nd and 3rd instances.
Hope that helps,Owen SBusiness Systems and Configuration Controller
HWM-Water Ltd2 -
Well I tried that too, but I cannot select the first hole as 'Entity to pattern'. 'Part 1', which is the whole cylinder, is always selected automatically. And the unasked question remains: how do I specify planes in arbitrary positions. The help menu shows several different plane generating methods, but I have no idea how to use them.
Anyway, thanks for your help.0 -
@hansrudolf - you need to change the first option in the Pattern feature - it defaults to Part Pattern - change it to Feature Pattern. For planes like "tangent to cylinder", you will need to create some construction geometry first. A better option for creating these types of holes is coming soon.Senior Director, Technical Services, EMEA6
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Have you changed the option in circular pattern dialog box that defaults to 'part pattern' to 'feature pattern or face pattern'?
https://cad.onshape.com/documents/7287b4e86e87c88d8064de6d/w/ec4fe057bbe02f84a273eb55/e/02c1174a849117e2eed21937
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@hansrudolf
You need to switch to "face pattern" instead of "part pattern", then the internal faces will be selectable.
I definitely think that patterning is the correct workflow for this case (if you really want the planes instead of just patterning the holes, you could feature pattern the first Plane feature itself to get those planes). But I understand the desire to know how to create these arbitrary planes manually.
This documentation has a description (with image) of what each of the plane types does:
https://cad.onshape.com/help/Content/cplane.htm
For this case I would use a "line angle" plane.
First, make a sketch of the point you want on the top of the cylinder, and make a line at that point tangent to the circular cap:
Then, once you have all the tangent lines set up, you can use "line angle" plane to make the planes you desire. First, change the type to line angle. Next, select the line in question. Then, notice that at the top of the screen, the program asks for an additional selection to act as a reference. In response to that, select the top plane of the cylinder. Finally, set the angle to 90 degrees. Repeat for each line you have sketched.
Here is the example doc:
https://cad.onshape.com/documents/ad2cb985cde5d9c74d995174/w/a35aa6256629c1224c1f50f8/e/056336850d997aecd30ba926
Jake Rosenfeld - Modeling Team1 -
Or another way:
Senior Director, Technical Services, EMEA1 -
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@hansrudolf @owen_sparks - placing radial holes is much easier with implicit Mate Connectors!
Or if you prefer, place one hole and use Circular Pattern.Senior Director, Technical Services, EMEA2 -
WHAT???? How long has that been there?
Thanks Neil. Also it's the weekend, you're allowed to forget about us for a few hours!Business Systems and Configuration Controller
HWM-Water Ltd1 -
Jake Rosenfeld - Modeling Team1
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Business Systems and Configuration Controller
HWM-Water Ltd1 -
Well I can only say thanks a lot to all of you! It is almost unbelievable how fast and competent one gets answers for any problem. And sometimes even answers which - as it seems - are new even for the experts!
I will spend some time to digest all that and try it myself. Yes, my problem is solved by using the feature pattern.
Many thanks, and a nice weekend for all!
Hansrudolf0 -
Sure thing, it's like that here.
Owen.Business Systems and Configuration Controller
HWM-Water Ltd0
