Hi, I would like to pattern on a non planar surface as you can see on pic. How can I do that on SW2014? I attached the part file. Than you so much.
I have been trying to think of a way to do this and I can't come up with anything easy. My first instinct was to use the wrap/deboss feature to cut the grooves, but if the grooves need to be tapered at 90 degrees as it appears they are in the photo then wrap won't work. The best suggestion I can come up with (which isn't that great) is to model the knurled surface flat creating the grooves with a pattern of straight cuts. Then use the deform tool (curve to curve maybe) to bend the flat body to the final shape. Then you could trim it to be the exact shape that you want. I briefly tried to do this but I couldn't get the deform to do what I wanted (bend in 2D only).
Maybe someone else can think of a better way to do this.
As Jamil noted, there's more to that than it seems at first glance. I didn't try and replicate your part exactly, but the procedure might work for you.
I used a swept cut, first circular patterned (mirroring works too) then linear patterned. Note how the initial cut overlaps the final surface size enough that the final pattern covers the entire part. Have a look at the model and see what you think. Some of the problems I noticed are that the checkering grooves are not perpendicular to the surface as it curves up and down. If this is important to you, you may need to play with adding guide curves and/or try making multiple cuts with the groove angle set appropriately for each cut. You would most likely need to make some of them asymetric for best appearance. It depends on what your requirements are.
Also this will only work if your part is uniform in section, if you have a compound curvature, you can use the same swept-cut method, but without the linear pattern. Each groove will have a unique path, fiddly, but not that hard once you get the routine sorted out. Depending on the shape you could probably do all of one direction and mirror.
Whatever you do, you will undoubtedly need a bit of trial and error. So, unless you have a very fast computer, keep your checker pattern course until you get things all worked out, you'll save yourself a lot of rebuilding time.
Yes. I've been seen your model you've performed many tricks in it. it's a good model and a good idea of creating model. But the process is too lengthier. There is an another way to simply create the model in a easiest way. It's in new feature in SOlidworks 2015 what's new "Variable pattern". See the attached video zipped file.
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This is a pretty good result. One thing that is not perfect about it is that the diamond pattern does not really wrap around the hump, it is projected onto it. So if you look at the pattern on the side of the hump the diamonds are elongated a bit. This would be more obvious if the hump were steeper (see image below where I changed the hump shape). However I don't know how precise the model needs to be, so this may be good enough for what Yusuf needs. It definitely looks good.
I'm glad you played with the profile. One reason I made it with a spline instead of just lines and arcs was to be able to see how well the cuts would sweep over various profiles. You can also change the square "checkering" to diamond shapes. I was surprised at how well it worked actually.
Your point is well taken, but as you also mention, without knowing more about exactly what Yusufs requirements and design intents are I hesitate to get too carried away.
Erik, thanks for your helpful asnwer. When I try to make this drawing from begining, it's really good way but I need to draw this pattern on an existing parasolid import geometry. I will also try your method on my existing geometry. Thank for your help again.
Working on imported geometry could get interesting. Keep us posted on what you come up with, and any hiccups you encounter.
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