Bending a flat pattern part into a cylindrical part 3

[3fguy]

Hello,

I just discovered this website today and am glad to be able to read all the valuable info that you put on.

That said, I have a question / problem im having. I have to create a cylindrical part shelled with a certain thickness(1.5mm). The cylindrical surface has an extruded pattern on it and it would be too difficult to create it as a cylinder and then extrude the patterns. The part has 3 repeating patterns of 120 degrees and thus, I have been successful creating a third of it as a flat pattern and then using the flatten and process bend commands to bend it to 120 degrees. Then I use a circular pattern and create the whole cylinder.

The problem is that I need the part to be exactly a certain diameter, in this case 23mm. Unfortunately, I am having a problem getting the flat to bend to exactly the diameter I want. It gets close, within 2-3mm but I need it closer. I realize this is because of bend radiuses and k factors and such.

Any ideas of how I may be able to do this?

Thanks a lot,
Ian

 

[Beggar]

Well, I'd do it the way that you thought too difficult.

I'd extrude the thin-wall cylinder centered on the origin leaving a tiny gap (.0001") so that I could unfold it as a flat pattern. I'd then extrude the pattern from a sketch on one the planes parallel to the axis and then pattern that/those feature(s) 120° about the cylinder's axis.

What about your features makes that procedure too difficult?

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[engAlright]

If your pattern is embossed you won't be able to unbend/bend the part, since Solidworks can only make sheet metal out of a part with constant thickness.

If the pattern is cut through the part, one idea is:

-draw the profile of your cylinder than do an "Extrude Surface"
-draw the sketch of your repeating pattern on one of the principal planes AS IT WOULD LOOK IN THE FLAT
-use the "Wrap" feature to scribe this flat sketch on to the surface
-delete the newly scribed out surface
-thicken surface
-insert bends

Hope this makes sense - an example would probably be a little more illustrative.

 

[3fguy]

Thanks for the replies.

I will be honest, an example would be a big help to visualize this. Beggar mentioned to leave a .0001 gap in order to unfold. This part will be machined from delrin(for now) from the SW parasolid model that I provide the vendor with. Im not familiar with the machining process and wonder if the gap would be a problem when they load the solid model into their translation software to their CNC.

engAlright, I think I understand what you are saying but have not used the wrap command before. I can give that a shot and see if I can do something with it.

By the way, a picture is worth a thousand words and I can send anyone a pic of the part Im trying to do, should anyone care to see it.

Thanks for the help!!

 

[aamoroso]

If the gap is a problem, create two configurations, supress the gap in one of them for machining but keep it in the other for flatening.

 

[engAlright]

can you post a JPEG of the part you are after?

 

[3fguy]

Good idea aamoroso.

engAlright, I can post, but have to work on what server or site to put the photo. Any ideas?

 

[saltech]

Here is what you do
Create a sketch - your circle with its dia.
The center is at the origin.
create a construction line from the origin straight up.
select this line and turn on your mirror tool.
Drag a new line from the origin out at an angle past the circle boundry.
trim the circle between the mirrored entities.
You can turn off the mirror tool. Dimension the angle of the mirrored entities- say 1 degree.
extrude as a sheetmetal part.
Useing the unfold tool select the edge of the slit created as the fixed plane.
Create your cuts
fold back up.