Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
2. Need support? Ask a question to our Community Support category.
3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

# Hole perpendicular to a surface without a suitable plane

Member Posts: 12 ✭✭
HI all
I need to make 4 holes in a disk.
I am unable to create the holes perpendicular to the curved surface because I can't find a suitable plane.
In the document I am providing I created the holes using the top axis but as you can see they are on the right spot only on one side.
I would need a surface parallel of the surface of the disk. How can I achieve it?
Excuse me for my bad English I hope you'll understand what I am trying to explain.

Andrea

• Member Posts: 1,061 ✭✭✭✭
@andrea_rossi972

The most important thing was that I centered everything around the origin

It’s a good thing to center everything on the origin. This program will work best for you if you do

Check all the dimensions

See if this is what you want

I could not check them against your image because it was too dark for me to read

But if you make a section of this part you’ll see that it’s a lot cleaner than what you had. There’s more parallel lines. Things are tangent. That type of stuff

• Member Posts: 526 ✭✭✭
Here is another solution, Plane on a line angle

• Member Posts: 2,242 PRO
There are a number of ways to get what you want. If you really need to use the hole feature (as opposed to an extrude or revolve), then you may need to do a little more work. In any case, a sketch plane through your main axis of rotation can be used with the intersect sketch tool to get a linear edge for the top intersection. Then pick a point on that line for the center, and create a centerline perpendicular to that intersection line if you want to do a revolve

You could also use MultiMateConnector with the Face/UV options to create a Mate Connector in the right location, normal to the surface.
• Member Posts: 12 ✭✭
I really don't need to use the holes feature, the easiest and simplest method would be the best for me.
As you easily understand from my question I am a total noob and I use Onshape mainly for creating 3dprinted simple objects.

I found in the forum a possible solution using a script. I made a hole with this script but I'll try to replicate what you suggested to me in the future. Thank you
• Member Posts: 1,061 ✭✭✭✭
@andrea_rossi972

Multimateconnector is one of my favorite tools

here’s another nice tool along these lines
Surface Tangent Plane

• Member Posts: 12 ✭✭
Thank you all for your answers , I have a lot to experiment :-)

• Member Posts: 1,061 ✭✭✭✭
@andrea_rossi972

The most important thing was that I centered everything around the origin

It’s a good thing to center everything on the origin. This program will work best for you if you do

Check all the dimensions

See if this is what you want

I could not check them against your image because it was too dark for me to read

But if you make a section of this part you’ll see that it’s a lot cleaner than what you had. There’s more parallel lines. Things are tangent. That type of stuff

• Member Posts: 12 ✭✭
edited June 2022

Thank you very much for all your work. I am a total nob and your help is greatly appreciated. I realized my big mistake in not centering my first sketch to the origin but I didn't know how to move it, then following your input a learned the transform function.
Your model is almost perfect, I only need to move 2  of the 4 holes on the internal surface but I should be able to do it by myself now :-)

I had a lot of problems using the spline function because mixing it with "line" I always come to an unclosed surface. I worked around this problem by making a singular spline line and then adding lines inside it .I also noticed that you perfectly defined my section before sweep I have a lot of difficulty defining splines.  I am ashamed about how my project was badly made :-)

• Member Posts: 526 ✭✭✭
Here is another solution, Plane on a line angle
• Member Posts: 474 PRO
@andrea_rossi972, following @steve_shubin 's advice to layout your part symmetric to the origin will make your task vastly easier.  That is a critical best-practice.  Also note that a REVOLVED feature is a great alternative to SWEEP for your application.

I started by applying the "Offset Surface" tool (with ZERO offset) to create a dummy surface on the surface to be drilled (Offset-Surface is a seemingly simple, but super versatile tool with myriad uses).  Then SPLIT that dummy surface with a plane.  Refer to the simplified example in Part Studio 2.

Then use the HOLE tool, instanced to a mate connector rather than a sketch point.  The mate connector can be initially located to the center or either end of the split line.  Edit the mate connector to offset along it's Z-axis, to the desired location.  Then ROTATE the mate connector 90 degrees about the appropriate axis (x or y).

Hide the dummy surface and call it done.  Clear as mud?
• Member Posts: 12 ✭✭
Thank you very much for taking time answering me great suggestions