Cutting Corrugated Tin - Need Help

[JJsCustomDesigns]

I took on an order for 270 pieces cut out of Corrugated Tin. I didnt give it a second thought. I figured i have THC on my machine and it wouldnt be problem. I start with doin a few sample cuts on a piece of scrap and quickly realized my torch was not following the contour of the tin. I called PlasmaRoute to see if they could help me out. They said i need to adjust my settings and it will work fine. But they didnt have time to go over it with me.

Does anyone know what "settings" need adjusted?

I run SheetCam and Mach3. PowerMax 1250 Plasma Cutter with HandTorch

[sodfarmer]

I'm assuming that your machine has CandCNC controls. You probably need to go into the settings tab in Mach 3 and adjust your minimum thc rate, which is in a box called corrections. From the factory the default is -.125". So I wouuld adjust that number to what ever the height of the rib, in a negative number. You will probably have to play with the number. Hope it helps.

[JJsCustomDesigns]

I looked in the Setting tab like you said. The (-) number is already at -1.00. The rib Is right at 1.0"

Ill play around with it see if i can make it work. Theres also a THC % there.... its at 15%. Is that the amount the Z axis moves when the other axis are at 100%?

thank you for your response

[sodfarmer]

I can't answer the THC % question I have mine set @25%. I think this was the default setting that was installed when I built my machine. I would try that. I would recommend joining the CandCNC support group. Tom will help you if its his compenents, even though you bought the table from PlasmaRoute.

Link:
http://groups.yahoo.com/group/candcncsupport/

[vmax549]

I think you are refereing to the THC% which is the % of rapid speed that the Zaxis actually moves at. Get it too fast and the axis will stall and loose steps, too slow and it cannot follow the changes in Zheight accurately and will lag behind XY on fast cuts and large variances in Z. LARGE arc gaps causing poor cutting results.

Just a thought, (;-) TP

[vmax549]

Also good Corragated cutting require the PROPER feedspeed DESIGN of the Z axis Get the ratio of speed vs Torque wrong and you are limiited to HOW fast you can acutally MOVE the torch without stalling or causing Occilations in Z where the THC can no longer keep up with changes.

(;-) TP

[Dennis]

I called PlasmaRoute to see if they could help me out. They said i need to adjust my settings and it will work fine. But they didnt have time to go over it with me.

Nice customer support , They got your money and now your on your own....

[JJsCustomDesigns]

Finally got a few minutes of PlasmaRoutes times... In Mach3 you have to goto to "Config" - Motor Tuning - then click on Z Axis. ive been playing around with the Acceleration and Velocity. Still need to tweek it a little to get it working right. Seems that 35 ipm is too fast and 25 ipm is too slow. PlasmaRoute told me that I was going to have a really hard time with my HyperTherm 1250. I told him " If your machine can do it, so can mine". Ill get it tweeked around and post the results.

Ive wrote down everything setting i changed and what the default setting was.... Heres the kicker. I was cutting a few artsy things on Sunday and realized my torch was not rising after a cut. It stayed at cut height and rapided across the table. I ve had this machine almost 2 years and its never done that til a few days ago. I restarted Mach3 from 22 sessions ago. Still not fixed. In the begining of the G Code about 5-6 lines down it reads " "G00 Z0.000" . If i alter the 0.00 to 1.00 the torch will lift to 1" over 0" and rapid across the table before the first cut. After first rapid move it does not do this again. It stays at cut height and rapids across the table to the next location. Sometime it wont even touch off. Jus fire and go.

Any ideas?

[vmax549]

The THC's with Mach3 DO NOT use the accel values in the motor config to move the Z. IF you set the values too high you will start loosing step at one point and find you have the torch dragging the top of the material and will losose precise control of the Z when NOT cutting

Set the Motor tuning back to where it does not Loose steps. You adjust the motion of the THC's with the THC% setting. It is the %of rapid speed that that MACH3 will use when running the Z. Remember the Z will run as fast as the motor will run in accel. You are just controlling velocity. You you use the THC% to adjust the speed of the Z. AGAIN too fast and you loose steps and too slow you lag behind the XY and can't follow the height changes.

THAT said, MANY tables are built WRONG as far as the Z axis feedscrews for plasma use. THe idea movmen is 1" per rev of the motor. That is the best compromise of speed and torque for plasma and steppers on the Z axis is too fine then you can NEVER get the speed needed before the motors will stall and loose steps. GET it TOO course and you may run out of TORQUE with small motors to be able to Aceel fast enough and it still limits the speed. OR the Z moves TOO FAST and outruns the THC and then you get osillations where the THC is trying to keep up but can't. The Z is so fast it overshoots then corrects.

Those are the basic boundaries for the Z and THC control. Hope that helps, (;-)TP

SO that is about it in a nutshell. Hope it hepls

[JJsCustomDesigns]

alright.

Everything is back to factory specs, except the z rapiding across the table at cut height on regular flat 10 gauge steel. Ive tried the moving the THC % as high as 25% with very little change in torch motion when experimenting on the corrugated tin. Even at 25ipm. I was told by PlasmaRoute that do NOT go over 30% in THC Corrections.

[vmax549]

Well if they know their speed limitations and you still cannot cut the corrugated material then I guess you have run up against the limitations of the machine design.

(;-) TP

[vmax549]

It sound like your gcode is not correct. What cam are you using? May want to check the cut parameters in the CAM something may have changed in the tool table and it is no longer correct.

Can you post the lines in the gocde where it is suppose to lift to rapid height before it rapids.

Does MACH say it is at the correct rapid height but the torch is still dragging?

(;-)TP

[JJsCustomDesigns]

I'll post it tomorrow. The only thing i changed in SheetCam is i made a new Tool for the Corrugated material. I dont see anything in sheetcam refering to Z. All my cut & pierce heights are correct.

[JJsCustomDesigns]

Does MACH say it is at the correct rapid height but the torch is still dragging?

(;-)TP

Im not very advanced in reading G code. like i said bout 5-6 lines down from the start of the file it reads : G00 Z0.000. Then goes to pierce hieght, initiates arc, then to cut height and begins cutting that part. I found later in the code that there is a "PD0.00" after the cut has finished and its bout to move to the next cut.

Ill grab a buncha screen shots and post in the a.m. if that would help a little better.

[vmax549]

In sheetcam the Rapid height is set in the JOBOPTONS/ material. When you set up the materiall spec you set what the rapid height needs to be based on the material.

In the Gcode look after the M5 line whithin a couple of lines you should see teh Z retract up to rapid height

G00 Zxx.xxx (x's are numbers) if that shows Z0.000 then check the rapid height setting in Scam.

(;-) TP

[JJsCustomDesigns]

Ill check out SheetCam settings. Seems like i muffed something up in there. Thank you for you help. Ill let ya know if i got it fixed.

[JJsCustomDesigns]

I did end up changing Rapid Z travel in SheetCam. All good now.

I got my machine to cut the Corrugated Material. I returned all settings to factory in the Motor Tuning. I set the THC to 30%, running 60ipm @ 25 amps and 225 volts. Pierce height i moved to .1 and cutting height to .07. Seems to work good.

Thanks for helping me out.

[jimcolt]

Do you mean 25 amps at 125 volts? The Powermax1250 will not provide arc voltage above about 185 volts.

Jim Colt Hypertherm

I did end up changing Rapid Z travel in SheetCam. All good now.

I got my machine to cut the Corrugated Material. I returned all settings to factory in the Motor Tuning. I set the THC to 30%, running 60ipm @ 25 amps and 225 volts. Pierce height i moved to .1 and cutting height to .07. Seems to work good.

Thanks for helping me out.

[JJsCustomDesigns]

your right. I fat fingered it. 125 volts.

everything was working real good and all of sudden the torch will touch off.. initiate arc and immediately continue raise well above the material. until the arc is lost. im baffled.