Hole perpendicular to a surface without a suitable plane

andrea_rossi972

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.

https://cad.onshape.com/documents/da67d08339ce59ae305caa55/w/e9d889b32337dad52d44fee0/e/0cadf3ef595e0c9b98d22d6f


Andrea

steve_shubin

@andrea_rossi972

https://cad.onshape.com/documents/bbf0e60a4cba4ced8a4145a9/w/367efcd424bd51e3f2574daf/e/39dc30812feef1723cc36e6e

I cleaned up your sketch

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

dirk_van_der_vaart

Here is another solution, Plane on a line angle

S1mon

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.

andrea_rossi972

Thank you very much for your answer S1mon. 
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 read your answer many times but maybe the lack of knowledge of the software prevents me to replicate your instructions.

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

steve_shubin

@andrea_rossi972

@S1mon gives great advice.
Multimateconnector is one of my favorite tools

https://cad.onshape.com/documents/cbc5092b15def4c6ed0ff88d/w/8c890c1d32245dbc3a46af8f/e/4890614af469372ec6d5df91

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

andrea_rossi972

Thank you all for your answers , I have a lot to experiment :-)

steve_shubin

@andrea_rossi972

https://cad.onshape.com/documents/bbf0e60a4cba4ced8a4145a9/w/367efcd424bd51e3f2574daf/e/39dc30812feef1723cc36e6e

I cleaned up your sketch

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

andrea_rossi972

steve_shubin

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 :-)

dirk_van_der_vaart

Here is another solution, Plane on a line angle

matthew_stacy

@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?

andrea_rossi972

Thank you very much for taking time answering me great suggestions