Pattern of holes through a cone?

donovan_magryta

Hi,
I am trying to make a pattern of holes through a cone all going the same direction, but the fill pattern feature script doesn't seem to work with cylinders or cones.
What should I do?

Jake_Rosenfeld

Hi Donovan,

There were a couple problems with your fill pattern.  First, the edge specified for 'direction' was confusing the feature.  I drew a new edge that is just flat along the XY plane and used that for the pattern direction.  Secondly, the 'distance' variable is the distance between the centers of the pattern instances. Because the patterned face had a .07 inch diameter and the pattern distance was selected as .05 inches, the pattern would basically destroy the entire cone.

See my fixes here (feel free to copy my copy so you can see my inputs to the fill pattern feature):
https://cad.onshape.com/documents/32f6beb4f22dfbe345102357/w/66dc199acd7a867a4166822e/e/3d27eecff8c69762370e0313



In case you're still curious, when Philip says "normal" he is asking whether you want to drill at a 90 degree angle into the face.  The normal of a cone (looking from the side) looks something like this:

Sorry for the crude drawing.

https://en.wikipedia.org/wiki/Normal_(geometry)

chris_winters404

Hello,
Are all the holes going through or are there specified depths?
Stay awesome and have a great week!

donovan_magryta

The holes ought to go all the way through.

philip_thomas

'What should I do?" - please post a link to a document that at least shows what you are trying to do.
Are you saying that the holes are all normal to the face or that the holes have an axis that are all parallel to one another? 
This is where a document that at least shows the problem helps - users will copy it and show you their solutions.

donovan_magryta

Here is a link the document: http://cad.onshape.com/documents/e3eba1ef75af5ff851a54a2a/w/6f1353a463acb74d53c4ac87/e/4e39817483db0e6820ef80a8

What do you mean by "normal to the face"? Forgive my ignorance, but I don't understand what that means.   Imagine a 2d physical house window screen, but extruded into a 3d cone with the holes continuing straight up the z axis. or imagine a physical cone mounted base-downwards on a drill press and many holes bored through it straight downwards towards the base. That's what I'm trying to design using onshape.

Jake_Rosenfeld

Hi Donovan,

There were a couple problems with your fill pattern.  First, the edge specified for 'direction' was confusing the feature.  I drew a new edge that is just flat along the XY plane and used that for the pattern direction.  Secondly, the 'distance' variable is the distance between the centers of the pattern instances. Because the patterned face had a .07 inch diameter and the pattern distance was selected as .05 inches, the pattern would basically destroy the entire cone.

See my fixes here (feel free to copy my copy so you can see my inputs to the fill pattern feature):
https://cad.onshape.com/documents/32f6beb4f22dfbe345102357/w/66dc199acd7a867a4166822e/e/3d27eecff8c69762370e0313



In case you're still curious, when Philip says "normal" he is asking whether you want to drill at a 90 degree angle into the face.  The normal of a cone (looking from the side) looks something like this:

Sorry for the crude drawing.

https://en.wikipedia.org/wiki/Normal_(geometry)

mahir

I believe Fill Pattern can only pattern features on a planar face. Cones are not planar. If you want to pattern on a non-planar face you can try using a Curve Pattern. I have a Curve Pattern Normal FS that I created specifically to keep features normal to a surface. See below for an example and links.

FeatureScript Curve Pattern Normal

https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/5b92bac572d374d2da038f5c

Jake_Rosenfeld

@mahir The fill pattern works correctly on the cone as long as the pattern direction is set correctly (it can't create normal pockets/protrusions like the picture you posted though.)  See the link I posted above ^

donovan_magryta

Thank you Jake_Rosenfeld! that works like a charm.
I am having some new troubles though... I need to reduce the spacing between the holes and add a higher concentration of holes. Also, I need the exit holes (on the pointy part of the cone) to be exiting in a helical pattern like a holes along the thread of a screw, and enter on the flat side in a spiral or pattern.

Jake_Rosenfeld

Hi again,

I created a new Part Studio in my copy of the document called "Spiral Cone".  In this part studio there are two cones with spiraling bore holes.  Both use a similar approach:

1: Bore a hole through the cone
2: Create a spiral on the cone with the 'helix' tool: https://cad.onshape.com/help/Content/helix.htm
3: Start a sketch on the bottom of the cone
4: project the helix onto the plane (as a spiral) using the 'use' tool: https://cad.onshape.com/help/Content/sketch-tools-use.htm
5: Use a 'curve pattern' with the 'face pattern' option to bore similar holes along the spiral we generated in (4).

The only difference between the two cones in 'Spiral Cone' is that you created yours with a revolve, and I created mine by lofting between a circular profile and point 3 inches above it.  Hopefully this can give you some guidelines on how to start getting the geometry you want (draw whatever pattern you want in the base of the cone, and use curve pattern to bore holes).

https://cad.onshape.com/documents/32f6beb4f22dfbe345102357/w/66dc199acd7a867a4166822e/e/4c356f013703cdf2a7a18531

donovan_magryta

Hi Jake,
It needs to pack as many holes as possible along the spiral. How do I do that? It just gets wacky looking and the width between holes stays to far while the length gets squashed
http://cad.onshape.com/documents/4858ec47bb6b8594182dc626/w/2284800199f44f812e7e9f9d/e/0046c997f5f838a027159a76

philip_thomas

  Just for fun






https://cad.onshape.com/documents/b9dacdbfbbddef2327ff68d8/w/aadcaa5cacae62f3bee016b2/e/3d5a733065480eda2ed84b1b