Is it possible to multiply a feature in a part according to points from a sketch?

Sylvain_L

Hi everyone,
I would like to multiply a feature I need in several location in my part.
Is it possible to clone the feature to other places according to points from a sketch?
I am thinking about the feature "Sketch pattern" from Solidworks.
Thank you for your help!
Sylvain

NeilCooke

There is no built-in point pattern feature, but there is a custom feature - just add it to your toolbar using the + button at the top of this doc: https://cad.onshape.com/documents/9fca78cb66a0bc83e359eb3e/v/7b8e02af4e9b52af8d3ba60b/e/d7f44d3f530f6db8852edfeb

NeilCooke

There is no built-in point pattern feature, but there is a custom feature - just add it to your toolbar using the + button at the top of this doc: https://cad.onshape.com/documents/9fca78cb66a0bc83e359eb3e/v/7b8e02af4e9b52af8d3ba60b/e/d7f44d3f530f6db8852edfeb

Sylvain_L

Thank you for your help Neil, works great! 

mahir

Down side being the sketch pattern FS only works in part studios. So, if you later create a BOM, you'll end up with identical parts listed as separate BOM items.

Cris_Bowers

@mahir That's true, but if you have a part that requires a lot of identical merged features it's very helpful. For patterning a repeating part in an assembly I create a very shallow flat bottomed hole using this Blind Hole FS, https://cad.onshape.com/documents/7a6ed140dde321c090b9129b/v/ffd6ec5c049c1f348133763c/e/7e3539ae88daaaed0dd2a32f. I use it mostly for placing weld studs, but I could see it being used for other parts as well.You could probably just use the regular hole command to create a center punch, but we scribe the outline of the weld stud head on the plate so our guys can't mess up the positioning too much.

philip_thomas

Gentlemen, i may be a bit late to the party, but i come bearing gifts!

This custom feature (https://cad.onshape.com/documents/e02f8da5c872d4d55e30e218/w/41d8b64176967ea1955c14fa/e/78acc1887ae1c49f1407d251), is PARAMETRIC and allows you to being in parts from other part studios and other documents (using the new FS reference capability).
Because its parametric, if the sketch is edited, then more or fewer instances will be created.

It kicks a**!  

mahir

@philip_thomas, very cool. That's a nice upgrade to @cody_armstrong's point pattern FS. But there still needs to be better options for assembly patterning besides just linear and circular. On a side note, is there ever going to be something like FS capability in assemblies?

philip_thomas

@mahir - what options are you looking for? Have you submitted enhancement requests for these other pattern types?
With regards to FS for assemblies - we talk about it a lot, but nothing that I can state as being company intent. Let's just say 'never say never'!

MBartlett21

@mahir
Here is an improvement request for 'AssemblyScript'
https://forum.onshape.com/discussion/9663/featurescript-for-assembly

Cris_Bowers

@philip_thomas is there a way to make this work for features, like holes?

I have 22 individual letters in a part studio that I need to drill and tap holes into the back of. There are more than 100 holes total. Furthermore the hole feature keeps failing when I get to the 93rd hole. I thought there was something wrong with the geometry of that letter, but after further testing, it appears there is a cap of 92 holes per hole feature. Is that true?

philip_thomas

@Cris_Bowers - do you mean like this one?



https://cad.onshape.com/documents/4c1aba613a40947311bc6d05/w/3a2a6e89b11af1ac81749f98/e/16f4dcf95b4d67030e3eaa4f

Cris_Bowers

@philip_thomas No. That's working exactly the same as the hole tool except it lets you select the entire sketch instead of every point. It's having the same problem where it is failing because of too many holes/points. What I'm thinking is I need to place a single hole, then pattern the feature as a secondary operation. Your parametric part pattern is exactly what I need, but for features.

philip_thomas

@Cris_Bowers - so much going on here.

Parametric QLV's (the selection box) in all dialogs is something that we would like to do at some point - but that project is not currently scheduled.
So for now, any solution would be a custom feature (nothing wrong with that, they rock).
Your specific request (parametric pattern of a feature) does not exist as a CF currently (as far as I know). If I get bored here at work and no one is asking me to do anything, I could write one - but you can guess the odds of that happening.
That said, you can do it with the Parametric Sketch Pattern CF as follows.

• Make a dummy part in a part studio. 
• Make an in-place copy of the dummy part
• Create the hole you want to pattern in the dummy part.
• Subtract the dummy part (with the hole) from the copy of the dummy part
• (you now have the 'male' of the hole)
• Use the parametric sketch pattern CF to pattern the 'male hole' and use the 'subtract option'
• raise your hands in the air
• shout "Onshape rocks and Philip rocks!" (make sure you do it loudly)

Cris_Bowers

I was considering that option as well, I was just thinking the hole callout wouldn't work with it because it's a subtracted feature and not a hole. But I'll give it a try.

philip_thomas

@Cris_Bowers - no, the hole callout wouldn't work UNLESS, one of the holes on the plate was an original hole-feature hole.
Pattern the plug
Fill-in one of the holes (delete face)
Put a hole feature at the sketch point where the hole was filled in. 
Detail that hole in the drawing

konstantin_shiriazdanov

try this Transform pattern FS. it handles feature patterns

Cris_Bowers

konstantin_shiriazdanov said:

try this Transform pattern FS. it handles feature patterns

That doesn't work either. Only allows the holes to be patterned on the part they were created on

konstantin_shiriazdanov

@Cris_Bowers try to select multiple parts in merge scope when definining the hole feature

Cris_Bowers

konstantin_shiriazdanov said:

@Cris_Bowers try to select multiple parts in merge scope when definining the hole feature

That worked. But, I was able to reduce the number of holes to where I'm able to use a single hole feature now. I'll have to test to see if it will work with more. Apparently I counted wrong previously, because I'm sitting at 98 holes now even though I removed ~10.