convert tube to sheetmetal?

[dbcalo]

is it possible to convert a tube to sheetmetal? basically the shop wants some paterns they can attatch to the pipes to aid creation of discharge heads (pumps). so im thinking sheetmetal is the way to go. i've created the part but cant any of the sheetmetal commands.

also is it possible for the interference check to place semi-perminate lines to show where i need to cut? they wanted me to do this too but wasn't so sure it could.

 

[dbcalo]

my employer seems to think i can just run two pieces of tube together and have solidworks cut it precisely the way i want them, without make all the panels and references along the traditional way.

 

[ctopher]

Do a search here for "sheetmetal".

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[dbcalo]

ok. ran a search but nothing seems to quite fit what im looking for. it would be really easy if the dist head was a single part, not all round pipe, and not an assembly.

 

[ctopher]

Look for tutorials on sheetmetal. They have been listed here before.
Create your sketch, then extrude within the sheetmetal commands.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[CorBlimeyLimey]

A part extruded from a continuous circle cannot be directly converted into a sheet metal part. You will have to create a small gap in the sketch profile so that it creates a slit down the length of the tube. You should then be able to use the Insert Bends icon to convert it to SM. I find it easier to start the part as an SM part though.

However, if you just want a cutting line pattern, you can leave the pipe as it is and create a sheet metal part using the outside surface of the pipe:-
1) Select the outside surface & do an Offset Surface of zero.
2) In the Solid Bodies section, delete the pipe body.
3) Thicken the surface to whatever thickness of material you want to use for the pattern ... make sure the Merge option is NOT selected.
4) Create a small slit down the length of the thickened surface.
5) Select the Insert Bends icon then select an inside edge of the slit.
6) The thickened surface should now be regarded as an SM part & should be able to be flattened to create the cutting pattern.


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