Hoping someone in this forum can help me. I’m trying to scribe some parts on my crossfire pro but I want to do it with me manually setting the Z height and NOT using initial height sense. IHS adds way too much time and for the job I’m trying to do there’s a lot of scribing to be done. From what I can find, if I set the cut and pierce height to zero (I’m using SheetCam by the way) it turns off the IHS in the post processor. It does…. however it also disables all movement of the Z axis. I can manually set the zero height on the torch, but when I press go, the table starts running the program from what ever height the torch is at when I press go, and doesn’t move up or down. If the scribe is touching the plate, it starts cutting and never raises; if it starts 1” off the plate, it starts running 1” off the plate and never lowers. Not sure what the heck I’m supposed to do here. Any advice?
You can setup a new tool there is a plate maker in sheet can it what I used when I did the drawing of the dragon that is in fire share. Hope this helps
I’ve got the plate marker working, but it’s so inefficient with the IHS touching off every time. I want to turn it off and set Z height manually.
if you have sheet cam, in the machine type, also set up “Rotary tool”, then post process your scribe (like an engraver point tool). The M3/M5 would post the same for rotary tool as torch.
I’m not following how that helps eliminate the IHS. Can you elaborate, please?
You’re going to have to write your own post processor to do what you want to do. There is no easy way to set a Z zero and have the machine raise and lower the torch between cuts without using the IHS system.
OK,
Here is how to do it, I have attached also, a Sheet CAM post processor with the IHS code removed. You would load this PP for your engraving jobs, don’t forget to go back to stock for plasma. It is called, “FireControl-v1.6_Engraver.scpost” and it is in a “zip file” attached since the forum will not let me load the .scpost file extension natively.
(this one has some of my code that post into your g-code more tool data, as comments).
With this post you do not have to change sheet cam over to a rotary tool.
In sheet cam create a new “Plasma” tool call it something like plasma engraver. At any rate, once you create that tool. Then open up the “Tool Table” in sheet cam, and set your pierce delay & height to 0, and set your Cut height to what ever you want your engraving bit cut depth to be, for example “-0.01” or whatever you want your depth of cut to be. Just note this, that you MAY have to fool with that cut depth, since even with you setting that cut height, the IHS mechanical travel will still exist so only the weight of your engraver and head will be holding your engraving tip down. IF……. you want to avoid that, you might have to measure the actual full travel of the IHS and add that to your cut depth if the weight of the engraver and tool head is not enough to mark the depth you want. (Note, you will also have to manually turn on and off your engraver motor on your tool) (unless your scribing). Also, IF you end up adding the extra depth to remove the IHS travel, don’t forget to set your safe travel height for the tool that much higher so you don’t drag the tip. Of course “no offset” on your tool cut paths.
depending on your engraver tip (assuming a rotary tool), set you plunge rate to what that tool need to drill down into the metal before moving, same for feed rate.
Once you post your tool path, in firecontrol turn off IHS then import your gcode, it will bitch and say you have IHS enabled (since you have the IHS chip on your board), usual warning, hit ok. Take a look at your gcode, you will not see any IHS code in it. You will see the H0 since that tells Firecontrol that it will be controlling your Z-axis (not the THC).
FireControl-v1.6_Engraver.zip (1.4 KB)