Sweeping profile along projected to surface path

[dangartland]

 Hello,

I am attempting to apply a moulded pattern to the curved surface of a cylinder and repeat all over.

Flat Moulded Pattern

I am using the project to surface tool to create a path that I want to sweep with. When using the sweep tool the resulting body does not line up in some corners correctly. See attached screenshot.

Pattern applied to curved surface

I have tried using a guide rail but the tool will not generate. I have used lofting with rails and this does not result in the desired shape.

I have tried many options, including cutting a body to create the outline, sweep following a surface (which did not generate) and attempting to convert a flat variant of the shape into a t-spline but the body is too complex.

How can this be resolved?

[laughingcreek]

sweep is finicky sometimes. can you attache your exported .F3D file here?

[etfrench]

Most likely reason is your path geometry is not correct.  The center of the arc may not be on the centerline.  If you use a three point arc and create the endpoints accurately, the meeting points will be precise:

[davebYYPCU]

Works as Ed has demonstrated, when you have unfolded the cylinder in Sheet Metal, then refold for the finished version.

There are threads to teach you how to fold and unfold,  let us know if you get stuck there.

Might help.....

[dangartland]

Thank you very much for the reply, the flat model is drawn correctly because the edges line up when created flat. The problem only arrises when we attempt to use the project to surface tool to wrap the pattern around the cylinder. Only afterwards do the joins become misaligned.

Any suggestions?

Thanks again,

Dan

[dangartland]

Thank you for the suggestion to use sheet metal function. I have managed to use this to flatten the cylinder surface but when I attempt to join the moulded pattern to the flattened surface and then re-bend it the pattern does not remain connected.

I have studied the tutorial but can not find a fix for this.

Do you have a remedy for this problem?

Any further help much appreciated,

Dan

[davebYYPCU]

Ok, if you have the pattern on the unfolded cylinder,

it has to be Sweep / Extrude / Combine > Join (ed)

to become part of the cylinder as one body,

the refold will work but only as the original body.

How were you attempting to join the two?

[dangartland]

Okay, when in the Sheet Metal workspace and I have the cylinder flattened there is no option to use the sweep tool. The combine tool is not available either, so I tried to add a joint from the component version of the mould to the flattened face with no success. I also tried joining the mould to the flattened cylinder by join extruding which did not work.

Join to flattened cylinder

I tried using the Flat Pattern workspace, which has all the tools you specified. I used Sweep / Combine (extrude was not needed) to the flattened cylinder and exited the Flat Pattern workspace and nothing has changed. Is the Flat Pattern workspace only used for creating drawings?

Mould combined to Flat PatternHow can I join them together differently?

Thanks,

Dan

[davebYYPCU · Accepted solution]

After the unfold, 

jump back into the Modelling / Patch area, Design dependant, when finished in there, 

go back to the Sheet Metal and refold.

Might help...

[dangartland]

You are correct, I used the Modelling workspace and combined the mould to the flattened cylinder and once unfolded the mould now stays shaped with the cylinder.

Successful join

I have to point out for others who may have the same problem is that this doesn't seem to work if combining a component to the flattened body, they both have to be bodies.

Many thanks again, I appreciate it.

Dan