New issue.. in Mach? Mabie a setting i dont know about...

[Mr Patches]

Hey guys. Well i have a small issue.. Not really sure where to look for the problem here... Im running win7 with candCnC blade runner. Sheetcam and mach3.. i recently upgraded my home computer to win 10 for my cad program ( inkscape) to create r14 files intead of r13 files that sheetcam could not scale correctly in inches.. So the r14 format fixed that issue... However since that change now i have to hit run after every cut in my mach program..

Everything seems normal up to the first cut. My torch finds the plate raises for touch off and fires. At this point it doesnt move but the torch is on and raming up amps. It will not move unless i push run. Then it takes off and makes the cut torch goes off. Torch rapids to next cut touches plate raises fires and doesnt move until i push run again... So thats how ive cut my last two cutouts... is this something in sheetcam? Did i flip a switch some how and alter the gcode.... ?

[Thor]

Sounds like single step mode in mach3, should be a button to turn it off iirc

[Mr Patches]

The single step button on mach i have only lets my machine do one gcode at a time one line at a time. So is there another adjustment that singles out moves per cut? Because the g code runs the full cut when i hit run until the next touch off...Then it just sits until i hit run again..

[Larry83301]

Could you post a section of code so we can see if something in the G-code is wrong?


Larry

[Mr Patches]

Yes sir. I will load up a part here. Thanks Larry. Good call.

[Mr Patches]

Ok here is my gcode for the first touch off start. And where it sits with the torch on and i have to hit run to continue. After each torch start..

[Larry83301]

You are highlighting the M03 is that where it sits each time it stops on you?? If so it could be a drop in air pressure causing the problem. Just a guess, but an easy one to check.

Larry

P.S. I don't see anything wrong with the G-code.

[Mr Patches]

Thanks Larry. Yes sir. It sits there at each M code. Until i press run.. Other than that it cuts fine each time.. While it sits there it ramps up the volts past my set cutting volts so i try and hit run when it matches the set volts i have for the cut each time... it doesnt seem to be hurting anything yet however im kinda nervous about cutting thinner material this way. Incase im not fast enough on the run button and it burns larger lead in cuts from the volts running up past my set voltage... The air is good. The cutmaster 82 hasnt given me any low air readings.. Thank you for looking at the gcode though. I appriciate your time... ill call the manufacture and see what he thinks may be going on here..

[WyoGreen]

I'm pretty rusty on G-code anymore, but doesn't the next line tell Mach to pause? (G04 P0.2) Perhaps that pause is what's messing things up. Or maybe you're not getting an "arc ok" back to the controller.

Steve

[Mr Patches]

Mabie thats the issue Steve... hmmm. I need to find out how to break down the G code... i just ran it again and it does the same thing after each cut...

[Larry83301]

Mabie thats the issue Steve... hmmm. I need to find out how to break down the G code... i just ran it again and it does the same thing after each cut...

Exactly which line is it stopping on, is it the M03 or the G04? The M03 tells it to turn on the torch and the G04 tells it to pause for a specific time period. Neither of these should stop the machine completely ( unless you have single step turned on). Does it stop at the end of each line or only when the torch comes down at the start of each cut?


Larry

[Mr Patches]

It stops at the start of each cut Larry. When i do hit run its in position to cut so it takes off and makes the complete cut each time. Ill run a cut today and find the exact line its pausing on and write it down... ive set my peirce time to 0 in my tool sets. And step mode is off in mach so im not really sure what is going on... A friend of mine said the G code its putting out looks like a rotary tool code set...

[tnbndr]

A friend of mine said the G code its putting out looks like a rotary tool code set...

Possible because I think that with a rotary tool set it pauses after start to wait for the cutter speed to ramp up. Ran into that while setting up my pen marker setup.

[Mr Patches]

Roger that tnbndr. So i went into gcode edit and we eliminated all the G04. P02 thru P04 codes just to test and see what happened. Whaaala. No pauses. The table ran thru the full cut uninterupted... Now if we change the post processor i wonder if we can eleminate the P0 codes from being generated?

[tnbndr]

Your tools in SheetCAM should be set up using the Jet cutting process not rotary.
Perhaps changing this setting in your SheetCAM Machine Operations will help.

[Mr Patches]

Ok tnbndr. Thats what i was looking for. I couldnt remember where i saw that at. I will check that this morning and see what im setup on. Im hoping it says rotory cutting! Lol. So i can change it and loose those PO codes.

[acourtjester]

As tnbndr says create tools for different types of operations, then select that tool in the different operations. Doing this will show labels in the G-code and help to ID where or when a problem happens. Also different tools have different options like pierce operations not needed in routing. Routing operations have repeat area movements with increase depths of cut over the same areas.