F360
Sheet metal
Trying to slot out the bend lines for forming. In Design, when the part was modeled, I unfolded the sheet metal. Then, I drew a new sketch using the largest face as the sketch plane. Projected the bend lines, and modeled two vertical slots, extrud cut the two vertical slots.
The modeled part looks correct. However, I can not get F360 in Manufacturing to allow a tool path inside the two vertical slots. I get an invalid linking warning.
Even started from scratch and tried two different-sized vertical slots, Zippo. The modeled slotted hole features cut fine, just not the slots.
Part as modeled:
Bend line slots projected and added:
Manufacturing fail:
Do I need to project the whole flattened profile and make a new part to the slot?
It is all about the lead-in/lead-out. There needs to be room. If there is not enough room then Fusion will disregard it. Just to show that it will work, remove the lead-in/lead-out and see if Fusion calculates a cut path.
That slot is about 0.1 inches and your lead-in is about 3x that. Reduce the lead-in to something like 0.03 or even smaller. It might be a little ugly but it is for bending, not for admiring.
If it still doesn’t “take it” you may need to give Fusion a “Preferred Lead-in Location” on this tab. In this example, it would not even be worth trying the “preferred lead-in” because I can tell it wouldn’t fit:
The best way to cut bend lines is to just use a single line in the sketch. Cut the line with no offset and turn off lead in/out and set pierce clearance to zero.
If you extrude the slot, it makes a loop that requires enough clearance for the torch to pass in both directions.
@ChelanJim Great info thank you. I made this post, then a follow-up with another screenshot to show I had removed the lead in and lead out for the bend slots but was still having the issue. However, as a newbie trying to post on the forum for the first time on a weekend, I was locked out until a mod allowed my new post to go live.
I like using a radius for the lead in vrs the 60* straight line option I have started with.
Thanks for the welcome! Fusion 360 is new to me, coming from Solidworks.
@Kwikfab ok you just darn’ learned me what my issue was. I did not understand that the “Pierce Clearance” was the offset from the cut line! I thought that was something to do with pierce height. man that was it.
Like @ChelanJim said, it was a lead-in issue. Its me thinking the whole point of a lead in, is to move the piercing point away from the wall, then lead out to round out the move. Not a second, and additional distance from the cut… its the lead-in for the…well lead-in, thanks, Autodesk.
Ok got it. That also answers my other question on how to cut just a straight line!
@Kwikfab I like this. Make a center line between the two bend lines to run the torch down, and have “both” lead-ins set to zippo. Perfict.
But yeah many of us have done the single line cut for a bend relief.
Make sure you do those on their own profile so the rules don’t apply to your other geometries.
I only mentioned bend radius because you mentioned using the flat pattern feature - this takes into account thickness steel as well as other parameters you put in place. This is especially important if you’re making something that has to adhere to specific dimensions for fitment.
Using a long bend relief like that can cause your metal to crack if too close to the edge, although too short of a cut will give you problems bending it and could cause warping. Then there’s also the issue with throwing off your dimensions as the metal will “fold” over itself on the cut edge.
Just throwing this out here if accuracy is the goal here. It always is for me.
man that was it.
