(SW) pattern on curve surface?

I’ve been trying to do a hole pattern on a curve surface and I end up with distortion on the curve surface since Im sketching the hole pattern on a planar plane and it cut through single direction, what Im trying to achieve is a sketch that follow the curve (like the photo) any idea to do this on SW? any suggestion is appreciated :smiley: thanks!

You can try using the sheet metal tools for this application, start out from a flattened model and add your pattern. Then bend it into 3D using the sketched bend tool.

I’ve made a little example here:

Be aware this isn’t magic, if the pattern is too complex it won’t be able to bend it. But I think it can take quite a beating before it fails on you, certainly if you don’t need to re-flatten it. But that’s just a hunch :wink:

great tips in doing it in sheet :slight_smile: any clue to do it on solids?
IMG_3179 [640x480].jpg

Did you try some sort of pattern? Along curve or or what have you… If you fail to pattern the cut feature, try pattering solids, then combine>subtract them.
There’s also a wrap feature, I think that could be applicated for this.

You can also do a vertical section of that box with extrude tools, then pattern it along the X-axis, it looks repetitive.

You may try modeling the main form in solids, without any pattern cut into it. I would make multiple bodies of each separate panel by unchecking “Merge result” when making the features. Then convert each body to a sheet metal so you can unfold it, add your patterns with a simple cut-extrude, then fold it back.

You can probably also avoid having to make all of it, mirror things around and over when possible :slight_smile:


if you need something like that i can send you a link to download this file

i made it with :
First a repetition along curve , and the curve i’ve use is an composite cure.
Secondly one linear repetition perpendicular to the composite curve
Finally 3 symmetry to have the complet object

Looks good from the pic, jack! :slight_smile:

thanks for all the tips guys :smiley: !
@jackdark if you dont mind can I have a copy of the file so I can dissect it to have a better understanding? thanks in advance

won’t you have undercut issues with this pattern? Will you be designing inserts in the tool?


Are you ready for the dissection?

3…2…1… GO!


This file is in sw2010 I hope that you can open it.

By hoping to help you a little


Ps : sorry if my English is bad, i’m French, i’m working hard to learn this language

thanks jack!

guess there’s more than one way to skin a cat. you can pattern your features and use a boolean operation (combine subtract)

That’s a great idea, make the bodies extend nice and through the main solid you want to cut, unlike a feature curve driven pattern a boolean subtract with nicely overlapping cutting bodies won’t be even nearly as picky about end conditions that might cause the feature to fail.

This last method looks interesting - beanworks can you please break down the features a little more for this SW user? What is the Boss-Extrude doing?

yes, please break it down :smiley:

sure. The boss extrude is the oval piece I patterned and used as the cutout. Then I patterned it along one edge of the surface. Then I crvpattern the row of oval pieces to follow the surface. Then the surface was thickened to make it a solid. Last, I did a combine (subtract) and subtracted all the pieces. Its not going to be the best way for some situations but it will guarantee a pattern thats normal to the surface.


I think one of the things that you might consider is that right now you are modeling it the way it will “end up”. “If” and this is the “X” factor, “if” this is a uniform wall thickness then you might be able to get away with it as a Sheetmetal part. Being able to flatten it out, cut the pattern, and then roll it back might be an alternative way to skin this cat…

I’ve seen people use this same thing for cardboard layout