Mastercam 2018 Part to sheet metal pattern

Hello. I could use a little help. I made a model is SW 2018; I made a model, and used the shell feature to end up with a "sheet metal" part. What I would like to do if possible, is to take my model, and flatten it to obtain a DXF....is this even possible? Thanks. Mark

Have you tried using the Unroll C-Hook?

Unfortunately, I am not familiar with that, or how to use it...

SW 2014 here so 2018 may be different. I think the latest version I've used is 2019. With sheet metal parts there's a "Flat Pattern" feature that's created automatically but it greatly depends upon how the part was created. The "Flat Pattern" is the bottom feature in the model tree and it's suppressed. Expand the feature (+) right click on the mouse on the "Flat Pattern" (try one or the other) will give you the option to un-suppress it and lay it flat. Very often a part created in solid modeling may convert to sheet metal but not be able to generate a flat pattern. The sheet metal module operates a bit differently than solid modeling. Solid models converted to sheet metal need a fixed edge/surface as a reference for all other features to "unbend" around, sort of like it's an axis for rotation/unbending. The program needs something fixed or it has no idea what the reference "zero" is.

Last night I wanted to create a sheet metal cone that had a 16" OD on one end, a 12" OD on the other. Most attempts ended with a flat pattern that was simply a rectangle, this was clearly not correct. Finally creating it as a loft generated the correct flat pattern.

My point is that just because the feature tree show the part as being sheet metal doesn't mean it will have the flat pattern you need. It really depends upon how it was created and converting solid to sheet metal will often not work as intended. Without seeing your part (and the feature tree) I can't offer much more help. Have you ever run through the tutorials on the sheet metal module?

M. Roberts said:

Unfortunately, I am not familiar with that, or how to use it...

Click to expand...

When in Mastercam, hit ALT+C. This will bring up the C-Hooks folder.
I swear there used to be an Unroll, but I guess there isn't one anymore.
There is one called Rolldie, and another called Flattensurf.
Never used either, but they might work for your situation.

Mtndew said:

When in Mastercam, hit ALT+C. This will bring up the C-Hooks folder.
I swear there used to be an Unroll, but I guess there isn't one anymore.
There is one called Rolldie, and another called Flattensurf.
Never used either, but they might work for your situation.

Click to expand...

Roll/UnRoll is in Transform.

I'm not sure about Flattensurf, but Rolldie is for contouring rotary/axis substitution parts.

Odd workflow...
wasn't sheet metal part of even the standard version of Solidworks? If the model was created in Solidworks, then you simply convert it to sheet metal inside SW, enter material thickness, bend radius and pay attention to K factor, that will affect the layout dimensions, really easy to use, (from memory) click convert to sheet metal, then pick a surface on the part you want to be central-ish in the layout and just go around and click on corners to create bends. Once that is done, you can also cut/extrude where necessary. There will be a suppressed feature in the design tree, if you un-suppress it, you can see the flat pattern instantly, I think there was also a button that does that. Once everything looks alright - create drawing, insert flat pattern (paying attention to scale), and save it as DWG/DXF for laser or waterjet or whatever, I used to include at least one dimension in that file for reference, to make sure that whoever is going to then use that flat pattern file, can make sure that it is imported in the right scale.

p.s. don't try this with Fusion its sheet metal implementation is absolutely horrendous, everything is pretty much the wrong way around compared to SW

CarGuy90 said:

Roll/UnRoll is in Transform.

I'm not sure about Flattensurf, but Rolldie is for contouring rotary/axis substitution parts.

Click to expand...

Well then I stand corrected lol. I've never used Flatten Surf or rolldie.
But I have used roll/unroll, not often and since you mention it I remember now.

Which software is the OP's question? Title says Mastercam, but first post says SW... as in SolidWorks?

M. Roberts said:

Hello. I could use a little help. I made a model is SW 2018; I made a model, and used the shell feature to end up with a "sheet metal" part. What I would like to do if possible, is to take my model, and flatten it to obtain a DXF....is this even possible? Thanks. Mark

Click to expand...

Just go "save as" .dxf. It will give you the option of flat pattern with or without bend lines.

If you have a sheet metal part in solidworks create a new drawing (File - New - Pick Dwg Template), then insert a drawing view (insert - Drawing View - Model - Pick your model under part/assembly to insert box - hit next arrow button and select flat pattern under more views and then place it in the drawing window). This should give you the flat pattern, then do a file save and use the drop down to save as a DXF/DWG and then import the DXF/DWG into Mastercam. That is how I do it. IN some version so solidworks you can't unsupress the flat pattern in the part till you place it on a drawing.