Fill pattern FeatureScript

peter_wittrock

I can't find out how this fill pattern works. Can some please very simple explain how it works?? Please Help

mahir

Think of it like any other face pattern (as opposed to a part or feature pattern).

1) Select the faces of the feature you'd like to pattern.
2) Select the target face you'd like to fill.
3) Select an edge for the fill direction (pattern angle).
4) Choose your spacing/border

3D

Is the "edge" you select at point 3) the depth? 

NeilCooke

@3D the edge is the direction the pattern the fills the face much like a linear pattern. The depth would have been created in the original to pattern. 

tgunr

I still don't get it. I want to fill a circular solid filled with holes for a speaker grill. The fill pattern I try to use does not seem to like an remove extrusion.

https://cad.onshape.com/documents/b02eed5aefc335d563b8d440/w/906f5fc8757f68a424e35f29/e/f0839677a4a7db3c242ae762

NeilCooke

For circular patterns you can do it using variables and regular circular pattern. You need variables because the number of holes will change as the pattern radiates. You can see an example here

http://onshape.wistia.com/medias/xd3lxgwsf6

Jake_Rosenfeld

@tgunr

Maybe try @paul_chastell 's Fill Pattern rather than the "Circular pattern" feature that you're using?

https://cad.onshape.com/documents/580ac6963bfeb2844a03047c/w/0a8fa7b507f35cb00c9c3d72/e/b6c791f900c6253fd1127950
https://cad.onshape.com/documents/57361ad4e4b00e5012c3857c/v/eb8bfe2edd984a315033e6e2/e/14aa44d127806651b248b9c6

@mahir it appears that your "Circular pattern" feature isn't playing nicely with multiple faces here?

mahir

@tgunr, I agree with @Jake_Rosenfeld. My circular pattern FS probably is not the best choice if you're trying to create a true fill pattern. However, if a radial shaped pattern is your goal, here's an example correctly using my circular pattern FS. @Jake_Rosenfeld, seems to work fine with surfaces for me? You just had to check "equal spacing".

https://cad.onshape.com/documents/5422f3fba6539c3f00ecf19d/w/8e82a7ccc9ddfacab355652a/e/2a6792505cbaf44083c7a0e0

Jake_Rosenfeld

Thanks @mahir !

mahir

@tgunr, I added an example of using Fill Pattern as well.
https://cad.onshape.com/documents/5422f3fba6539c3f00ecf19d/w/8e82a7ccc9ddfacab355652a/e/2a6792505cbaf44083c7a0e0

tgunr

Thanks for the help but I am still not able to create a fill pattern on this simple example.

https://cad.onshape.com/documents/8210036e4f921a2b795c8339/w/0a1b6e46ee34f66b5f526baa/e/f36bb678d63af985f2f83eab

I finally got that the face to pattern is each face of the pattern and not the pattern itself, but when I try to select the target face I always get the face of the sketch and not the face of the extrude as in your example.

mahir

Try using Select Other. Alternatively, you can hide the sketch. You can unhide it later if you need it. 

mahir

Here's another functional example using the Select Other method.

https://cad.onshape.com/documents/4d38d6ef3778b931c452644b/w/ff297763de9a5f77b3943323/e/cec3ecf962427ce001e32fa5

tgunr

Bingo! Select other is the magic key to get to the extrude face.

tgunr

One last remaining problem in 

https://cad.onshape.com/documents/b02eed5aefc335d563b8d440/w/906f5fc8757f68a424e35f29/e/f0839677a4a7db3c242ae762

I need to create a circular pattern that is basically a cutout in front of each tab specified in Circular Pattern 1. If I set the merge for the extrude 8 to all then I can get a single cutout. But I can't seem to replicate the pattern since I am using Remove instead of New. Perhaps I am going about this wrong?

mahir

@tgunr, couple things. First, for a normal circular pattern that has no radial components or need to locate/center the seed, you can use the built-in Circular Pattern feature instead of my custom featurescript. Second, it looks like you were using a part pattern. There are three types of patterns.

1. Part patterns replicate solid bodies. This is useful when you have a specific geometry for the cutting tool, but not necessarily the resulting faces. After pattering you can use a Boolean to add or remove the patterned parts from your main part.
2. Feature patterns replicate entire features. This is how SolidWorks users are accustomed to patterning. It's user friendly but costs more in processing power.
3. Face patterns replicate individual faces. This requires more time up front since you have to select every individual face of a feature that you are trying to pattern, but it takes less time for the part to rebuild.

The fixed example below makes use of a circular face pattern. Take a look.

https://cad.onshape.com/documents/3cb973a1e944a9f6c2363c64/w/221de857c5277a55fc5db58e/e/4a74a676e37e44cbf1f47f4d

tgunr

Ok, I think I see what you did. I tried to replicate with normal circular pattern but can only find 1 "Extrude 8" face. How did you create and select the other faces?

tgunr

Never mind, I see it now.

tgunr

Just when I thought I understood this, now can't create a pattern of hexagons.
I select all sides (faces) of the hexagon  (as Extrude 2). Setting the target to Extrude 2 or the face of the sketch, neither works. Tried including the top of the extrude, no joy. I am obviously not understanding something but don't know what it is, and the error messages are not helpful at all. "Fill Pattern 1 did not regenerate" a why would help. 


https://cad.onshape.com/documents/e15706c550e8532550901d4b/w/ad0746f0bafda4feb91256a5/e/997d5c6166e867930c226015

Seems to work with a Extrude Remove but not Add or New

mahir

Yeah, this seems to be a limitation of the custom Fill Pattern FS - one of the reasons why it's still just a FS and not an official OS feature. It will only pattern surfaces that share an edge with the target surface and also go all the way through to the part. Depending what you want to do, you can likely get the desired results using a combination of the Fill Pattern FS, standard extrude/revolve, and various boolean operations. See my link below. I patterned the surfaces of a pentagon-shaped cut. Then, I extruded a tool body and added material to the target body. Using those bodies as inputs for a boolean yields the results below.

https://cad.onshape.com/documents/adad529fd2168dfd3f594607/w/d71925605c33ced9bc111bcb/e/5663ab85e357ef03b34f57ff