Has anyone been able to find a simple way to add bend relief cutlines in a part that uses the sheetmetal component? I have a simple pan that I want to cut reliefs in to make it easier to bend but cannot seem to figure it out because the body is folded, when you go to flat pattern you cannot extrude those lines. I am using the flange tool to create the sides so when I look at @TinWhisperer 's video or others I have found they don’t apply precisely.
Thanks
One day I do want to make a sheet metal video.
When I do it I use the unfold tool.
Then I lay a sketch over top of everything.
I project my center lines from the bend line.
That I use the slot tool in areas I want to provide relief.
Then I use a cut extrude.
AAhhh I was just coming back to upload a fusion drawing that I essentially stumble into that solution sort of… I can extrude the slots but not the lines. I suspect because the lines are not part of the body. This file has slots but I had to guess on where to place them. I see two line, in the flat pattern there’s the extents and the bend for a total of 3. How are you getting the bend line in the unfold?
Thanks!
box for bend relief test v1.f3d (144.9 KB)
unfolded pan v2.f3d (310.9 KB)
here one i made on my computer . seems to work. ill keep review my preferences .
Ya I can do that, it looks like your slots for in between the extends? is there a way to have it cut the slot in one pass though when it’s the same size or less than the kerf? That’s why I was trying to do it with a line…
Another way you could do it is create a DXF from the flat pattern open it up in a new drawing and I believe it gives you the option to have the center line and the extents of the bend line.
Extruded.
Then open up a new sketch on top of the extrusion.
Turn on the visibility of the original sketch.
Project the center line.
Then draw a single line on the center line the length you want to cut.
And then in manufacturing make sure you do a single line cut on center.
I’m up from my computer now but when I get back to it I’ll run through this scenario.
I would love if you did a video on this! This is something I want to learn. I know it’s a little clunky but till now what I have done is draw it up. Then save out a second sketch and do all the cam for the bend lines in a separate file . Then extrude the first file and do the cam for the body.
After posting the g code I cut the bend line file first then the body.
I watched your videos on projecting lines earlier today and am going to try these methods next time.
Thanks @TinWhisperer for the detailed instructions and thanks @ScottNH for asking the questions.
So I worked on this some more since this thread. Since we had this discussion I was always using the slot tool in F360 to create the bend relief as I have yet to figure out how to extrude a line (don’t think it’s possible). It’s not the ultimate solution though as the the torch runs over the area twice.
Yesterday I found a solution that is better and I think @TinWhisperer was illuding to it earlier in the thread but I was too dense to get it.
Simply add the lines via a sketch on the flat pattern. You can then select those as contours in the CAM workspace. I have yet to cut the piece but it seems to work fine in simulation.
The exact technique I use if I’m only cutting a single line is I make another drawing to take the line from.
My back is totally effed so I’m going to be in front of my computer for the next couple hours . I might do a few twitch videos and do this quickly.
I just lay the relief line right on top of the bend line in the flat pattern using a new sketch that I name bend relief lines.
I find that a single line( except in only the thinnest of materials) is too narrow for bend relief. For myself when making a relief on 14 gauge to bend at 90° a single line kerf width is too narrow so the material will crash before it bends 90deg.
@Erock89x had this interesting twist on making the slots for bending. In this demonstration, there is some information that is not viewable such as him inputting values in menu boxes but you get the gest of it. Basically, he makes the extruded flange in sheet metal then cuts a slot with extrusion in the flat pattern.
ill start in about 10 minutes
I’ll build a pan and do a single line relief then a slotted relief
Here is the F3Z file if you are interested to playing along.
Example Sheet Metal Pan v1.f3z (427.3 KB)
Fun one to watch…!! Thanks for filling in a bit of the afternoon for me! LOL
Thanks for the video. It is similar to the way I’m doing it. It’s interesting that there are a few differences in the dialogues from Windows to Mac in F360. Never really thought about that.
Just had a call with Autodesk support regarding these bend line relief cuts. The ways we are doing it were all this person knew to do. He did say he would put in an improvement request to add it to the sheetmetal tools though 
Im glad i’m not the only one looking for a more simple route, however this is the easiest way ive found thus far.
ive gotten alot faster at it.
dont forget to turn off lead in/lead out and pierce offset if you are using thin gauge metal.
most of my releif cuts get welded back up anyway.
I know you said it here somewhere but I can’t find it. Did you say you use the material thickness as your slot width? TY
A good rule of thumb is a slot equal to or greater than the material thickness. You could go the entire bend allowance like @Erock89x example and you’re super safe…
The actual amount sits a little bit less than material thickness I’ll see if I can find the math I worked up for it at one time.
This picture illustrates where the problem comes in. At the inner Bend we’re dealing with compression everywhere from the neutral line to the inside radius (the neutral line offset) of the bend and we need to not have material there so we don’t crash.
Ultimately the best way to go about it is to do a few test bends with your particular equipment with different slot with and find The Sweet Spot for you.
