Configurations Help Required

brian_pinder662

https://cad.onshape.com/documents/20b7ed88dc59162296b5eb8b/w/a27f60c38cdafae14413fc59/e/aef92d9dadf7f2cfa23c1440  
Once again need more help getting to grips with configurations. Seem to have lost plot somewhere, in the URL above I have a 3, 4, 6, 8, & 12 Blade face plates Which Originaly started as a 8 Blade. As you will see i am trying to add the holes to each of the configurations. Everything works fine with the the 8 & 6 Blade but goes haywire on the remaining 3, 4, & 12. Somewhere I think there should be one or maybe two variables but how to form & where to put them I am at a loss. I have studied Codys Webinar on configurations & variables for some time now which are great but don't seem to be able to put them into practice. If anyone can can give some advice and point to where I am going wrong it will be very much appreciated and enable me to move on.
Best regards to all Brian.

owen_sparks

Hi Brian
Is anyone already looking at this, if not I'll have a look?
Owen S

Cris_Bowers

I would delete Holes from your configuration table. Move Sketch 2 to immediately after Flange 1. Edit Sketch 2 and replace the Sketch plane with the face of Flange 1 on the formed part instead of the flat pattern. You will have to redimension it here. Remember you can view the sketch normal to the face by pressing "N" on your keyboard. You can also just use points instead of the circles and use a vertical alignment relation between your points instead of dimensioning both of them, unless the alignment is something that can change. Replace Extrude 2 with the Hole command. Delete Circular Pattern 3 because you won't need it anymore. When you're done it should look like this:

owen_sparks

Hi Brian
Is anyone already looking at this, if not I'll have a look?
Owen S

Cris_Bowers

I would delete Holes from your configuration table. Move Sketch 2 to immediately after Flange 1. Edit Sketch 2 and replace the Sketch plane with the face of Flange 1 on the formed part instead of the flat pattern. You will have to redimension it here. Remember you can view the sketch normal to the face by pressing "N" on your keyboard. You can also just use points instead of the circles and use a vertical alignment relation between your points instead of dimensioning both of them, unless the alignment is something that can change. Replace Extrude 2 with the Hole command. Delete Circular Pattern 3 because you won't need it anymore. When you're done it should look like this:

owen_sparks

Hi.

Copy of your file here:-
https://cad.onshape.com/documents/a65f94f77fe9628e24897756/v/be0801198748ccf3c6326c07/e/5f1acc8bff3eb1c4a5055c10


You'll see:-
(a) Just one config input now as if we want a particular blade count we'll always want the corresponding holes.
(b) Centre hole moved up the feature tree and used as the rotation axis for the patterns as the outside edges change reference depending on how many blades there are.

Also worth noting that the orientation on the flat pattern does not match the part window.  I accidentally drew on the "top" flange in the flat for the holes.  This turned out to be flange 4, so if I set the blade count to 3 it fell over.

Hope that helps,
Owen S.

owen_sparks

Dang it @Cris_Bowers

brian_pinder662

Thank you very much, Owen & Cris. Could have just copied your example which would have been easy but grasping why & how it works took a little longer. Can now progress to next stage.
 All the best.