How to make a ball with holes in arbitrary directions?

[thundergao]

I am a new user of Solid edge. I want to design a vacuum chamber. The basic shape is a sphere. I need to make some holes in the sphere which directed to the center of the sphere. How to make it? Bow//

 

[swertel]

To create your sphere, start with a revolved protrusion and draw a half circle with solid centerline symmetric about the global planes. Revolve it 360 degrees (full circle icon) and you're done.

Next, use the hole command and create a hole on one of the global planes. Extrude the whole through the entire sphere in both directions. You can then pattern this hole, create more holes on the primary planes, or create more reference planes at various angle to create holes on.

--Scott

For some pleasure reading, try FAQ731-376

 

[PhilDuron]

Hi Thunder,

You certainly created your basic shape as a "revolved protusion" using half circles (good practice is to center them at the intersection of the base planes) and revolving them 360°.

From there you mention you want all of the vacuum chamber ports to aim directly at the center of the sphere: one easy way of doing this is in using the "revolved cutout" command on an "angled plane":
- create an angled plane from the base planes (YZ and XZ typically) at the specified angle: this will let you easily adjust the port position further down the road when you start getting interference or simply want to improve the sputtering quality (or whatever you are doing in there!)
- start the "revolved cutout" command using this "angled plane" you just created and trace the "axis of revolution" starting at the center of the sphere and angled up or down at a specified value. Then simply draw the section to be revolved representing the ISO flange feature
- alternatively (for a welded port), you can also "revolve extrude" directly the feedthrough's profile still centered on the focal point and then remove the material that is left of the sphere inside the feedhtough using a simple "cutout" with the face of the feedthough as the reference plane and "including" the face of the innere cylinder as the profile to cutout.

Have fun!

Phil

 

[mascodesign]

TG,

Revolve a (closed) semi-circle to create your sphere, then use the Thinwall command to shell it. Remember to use DRIVING dimensions to control your Profile, otherwise you will have to re-enter the Profile environment and select the individual element any time you want to make a change.

To orient your ports, create a Coordinate System (UCS) for each port-axis required, then orient your Hole or Cutout using the 'Plane Normal to Curve' option and locking these to your Coordinate System(s) in turn.

REMEMBER to re-name your features in Feature Pathfinder (one of the panels in EdgeBar) for ease of navigation.

HTH,

Rick.