How to sketch on a sheet metal cylinder 3

[je696763]

Is there any way to sketch on a sheet metal cylinder while it is rolled, and then flatten the peice out and still have the sketch on it. I was thinking that there was a surface sketch or something that might work, but I haven't found it. We laser cut our parts, and if I have a sketch on it where something welds on I can have the laser put an etch mark to locate the tabs to be welded. Otherwise it is much more difficult for the guys in the shop to locate it on a part like this. I appriciate any help.

Thanks,
Jeremy

 

[SBaugh]

Look in the help

Use the index tab and type "Sheet metal"

The sub directory is "Cylindrical Faces"

It shows you how to make this.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[je696763]

Thanks for the reply Scott. I may not have been very clear in my description though. What I actually need is to make a sketch on the outer surface of the sheet metal part. I already have the sheet metal part created and need to weld a tab to the outer surface of it. I just want to make a sketch on the outer surface to locate this tab for welding. I'm just not sure if there is a way to do this or not.

Thanks,
Jeremy

 

[Dennyd]

je696763,

How about making some temporary or reference "points" on the cylinder that would represent the boundaries of the sketch and then unrolling the cylinder to show where they would be in the flattened state. I think you would have to make these a through cut such as a hole or rectangle. I don't think you can have just a set of points sketched onto a cylinder and have them unroll properly with the flat pattern. Conversely, you can put some cut features in the flat pattern and then roll the part to see where they lie, making adjustments to get them in the right place to line up. This latter method is iterative, but you can actually home in on the solution very quickly.

If this works for you as a work-around you might use configurations: one with the reference holes to determine where to locate things and one without the reference holes so you don't laser them into the actual part.

- - -Dennyd

 

[je696763]

Thanks Denny, that should work. I didn't think about doing it that way. I'll just make some cuts through it using references from the assembly and then flatten it out and make my sketches from that. Once I get that done I can delete my cuts and just have the sketches in the flat pattern. I appreciate the help.

Jeremy

 

[SBaugh]

I think I Understand...?

Could you not use a split line, 3dsketch, or a Wrap feature to scribe and area on your sheet metal part?

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[je696763]

Yeah, thats what I was looking for. It looks like the wrap command is what I need. I knew I had seen a way to put a sketch on a cylindrical surface, but I've never used it and forgot what it was called. I may be able to do it with a split line also, but I'm not sure how. I have already done this with the cuts, but I think I'll go back and experiment with this and try to learn something.

Thanks,
Jeremy

 

[je696763]

The problem with wrap, split line, and a 3d sketch is that when you flatten the part, the sketch on the cylindrical face is no longer is the same place. It doesn't move with the face as it is being flattened.

Jeremy

 

[SBaugh]

Try doing this - First use the unfold command add the wrap feature, etc... then use the fold command - see if that works.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[aamoroso]

Scotts last tip is a good one. Many people fail to see the power in flattening adding a feature and then folding again.

Another common option I use is to just sketch it in the flat configuration. We etch alot of our parts for an automated forming machine, the etch signifies the corner of the part to be loaded into the machine. We do this for most of our odd stuff like what you are trying to do. Our cam system was written in house and cuts all solid lines from our dxf files, problem we have is punched features. We create a second flat config that is outside of the drawing views the will be picked up by the cam software, the punched features are all suppressed there, the flat on the drawing shows all the features and thier dimensions.

Another option, odd as it may seem is usually the most simple, add a locating hole if you can, if the portion of the part is covered, in most instances a hole under a bracket is not a problem.