How do you slow down cutting out holes and other small pieces inside your material? Im cutting some 12ga at about 70ipm and the outside looks great with minimal dross but the inside smaller holes are a mess. Its a rectangle hole used to line up another piece of 12ga "tab" on the material and i cant get it to cut properly. Ive been messing with cutting that shape out on little squares and playing with speed and height and it doesnt get much better. The corners always have an inward bevel to them (the top looks square and the backside looks like a round edge)
guess i should have put the table specs: torchmate 2x2 manual height control esab powercut 1300 plasma 40a new consumables 80psi air 12ga material at 70ipm and i slowed it down to as much as 40ipm
If you go to Configuration > Machine > Feedrate Ramping you can change your Max Arc Feedrate this will govern how fast the torch travels around an arc. For direction change you can change Continuous Contouring, both of these should be about 70% of your feedrate. If Max Arc Feedrate is grayed out then you can click on Advanced and set your Centripedal Acceleration rate to .7.
this is what i needed to know! thanks. I changed the max arc feedrate but since its not an "arc", its a 90* turn, it didn't seem to do anything. I'll give this a shot and see how it does. is this something i have to manually set each run? It doesn't look i can set a percentage of normal feedrate, just a different feedrate.
so i have it cutting the inside parts way better but it leaves more slag. Not that big of a deal for a better cut quality. The only issue is that now the outside cut has slowed down to that same slow speed because most of the part has arc's to it. Is there a setting that always cuts the outside perimeter at full speed?
There are different ways to do this one is to create separate tool paths, for which most people do when they want the most accurate holes. If you had a base plate with 4 holes in it the normal plan would be to select all and make path then create male tool path. Instead you can select the 4 holes, make path (just to make it easier to select them) and create a female tool path (enter your feedrate on the Basic Tab) , then select the outside perimeter and create male tool path (entering feedrate). For instance you might set the feedrate for female tool path to 65 and your male feedrate to 100. Then do machine output in TM Cad, the Device for your configuration would be Torchmate Dual Tool Driver and the Tool of Multi-Tool. See the manual Multi Tool for TM3 and TM4 software. You could also create the male tool path as you normally would and edit the gcode once it is imported into the TM3/4 driver software. On our example the first 4 parts will be the circles so the initial feedrate governs those parts the F value at beginning of the gcode, scroll down to where the outside perimeter cuts and enter another F value for the perimeter, such as F100.
If it is just a few holes. You could edit the g code feed rate for those holes. Or change you max ark federate and continuous contour federate to 70IPM. If the machine is tight, it will hold. Also make sure you acceleration factor is 1.00
Or... you can assign a 75 in the feed rate for the interior cuts and 100 for the exterior cuts. Export it out of CAD as g-code and use the feed rate scale to determine the feed rate. Then your inside features will cut at 75% of the scaled feed rate while the exterior will run at the scaled feed rate.
Under Configuration > System > Controller turn off Express Mode then you can change the Max Arc Feedrate. Generally using Express Mode allows you to set Centripedal Acceleration Factor, a factor of less than 1 will slow the machine down on arcs such as .7 or lower.
