What do I save sheet metal parts to, for lazer cutting?

[Anonymous]

I'm not sure, but I thought, it would be a DXF.   I don't see an option for that.

Thanks.

[Breeze104]

Do you have ACAD?  I so create a dwg file and make sure you check the option to be able see it in the model tab.  Then strip all info and save as DXF file.  I have to save it as a ACAD 2000 ver.

Kind of a pain if you don't have parts already in ACAD.  If you do then just use that file and strip it down to layer "0" and defpoints and save as DXF.

[Anonymous]

No, I do not have AutoCad.  I do have BobCad 23, would that be any help?

Thanks.

[jtylerbc]

Our usual method is to create an Inventor drawing with 1:1 scale views of the parts to be cut, then export that drawing as either DXF or DWG (depending on the supplier's preference).

If you use "Save Copy As" from an Inventor drawing, both AutoCAD DWG and DXF formats should be available.  My guess would be you tried to do it from "Save As" instead, where they are not listed.

[Breeze104]

I totaly forgot about that.....  

One of those things I don't use, but I will be..LOL        

[JeffVN]

What we typically do is create a flat layout for the sheet metal part, then right click on the flat layout in the browser and select "Save Copy As" and you can save the flat layout as a .dxf.  You can do this from right within the part.

[JimSteinmeyer]

Another simular method is to right click a face in the flat state and select "export face as" this goes straight to a DXF.

[Anonymous]

Yep, that's how I ended up doing it, but my next question is, how does the shop know where to make the bend?

Thanks.

[jtylerbc]

You'll still need a detailed drawing with bend notes and such to tell them that.  The DXF is purely the pattern for cutting the blank material.

[JimSteinmeyer]

Agreed, drawings still need to be created. Otherwise how does the shop know what angle to bend to if they don't have a drawing?

Jim

[JeffVN]

Yes, we still make a drawing seperate from the DXF, as was said, they will need to know bend angle, radius, location.

One thing we do do though is have the bend lines come over in the DXF, and then instead of being on the "Cut" layer, we put them on a "Mark" layer.  We use a CNC Plasma table here, and the Plasma table is able to recognize the Mark layer as just making a light line in the part, instead of cuting it through.  This way the bend lines are marked in the exact location on the part, so when the part goes to the break, they have the location, and they just reference the drawing for radius and angle.

This is helpful on more complex parts that can be difficult to measure where the break line is, but will also just help speed things up in the shop, and increase consistency in the bends.   

[Anonymous]

How do you include the break line?

Thanks.

[Anonymous]

Also, does anyone know about the "paper" side up and or paper side down?  I know one vender who only looks at the dxf, with paper side up bends all of the folds down, or towards the nonpaper side.

Thanks.

[JeffVN]

You can select what layers you want everything to be on when you save the flat layout as a .dxf.  If you right click on the flat layout and select "save copy as", then assign a file name and location and hit save, you'll be brought to the "Flat Pattern DXF Export Options".  In here you can click on the "Layer" tab, and you can setup what lines you want to export to the DXF (Inner/Outer Profile, Bend Lines, Roll Lines, etc.) and you can also set what layer these lines should go to.  We have it setup so that the Inner and Outer Profile go to the "CUT" layer, and the Bend Lines (Front) and (Back) go to the MARK layer. You can also set your line type up in here as well.  

I would be careful about just assuming everything is bent towards the paper.  What happens if you need to make a "Z" bracket, or any other more complex shape with different bend directions?  This also doesn't get around specifying bend angles and radius's as well.   Unless you have very, very basic objects being bent, there are alot of assumptions being made, that can get you into trouble.  I wouldn't try to replace a properly made drawing.