Sheetcam or Mach 3?

[Oldsarge]

I'm finally getting to the part where I'm trying to do a test cut but I'm stuck.... I can jog, have all the axis moving correct distances, the torch fires when I click the fire torch icon. I set up sheetcam with the table dimensions, and the correct envelope size, loaded the correct tool, and operation. The drawing I load shows on the material correctly. I run the post, and then load the G code into Mach 3. I home and zero all axis, then jog over to where I have a small piece of 14 gauge on the table, and zero there, and set a reference point. So here's what happens:

In Sheetcam, if I run the simulation, all the tool paths are displayed etc, and when I run it, the torch just tracks off the table like it doesn't even know there is a job loaded.

If I load the .tap file into Mach, the torch drops hard, knocks the torch holder off, then takes off for the side of the table... I've tried with THC on and off, and have it set that THC isn't on automatically.

Very confused, don't know if this is being caused by Sheetcam or Mach3... I'm thinking Sheetcam since I can't even get the simulation to run properly. Also don't know why, when the switch is activated on the Z that the torch is still trying to drop more.... Thought it's supposed to sense the top of the metal that way then raise to pierce height? I hope this is just some settings I haven't found yet... Frustrating being this close!

Any help greatly appreciated!

Oldsarge

[I Lean]

Which post processor are you using in Sheetcam?

I agree, your problem has to be in SC rather than Mach3.

[Oldsarge]

I think the last one I tried was tge THC300 and I edited the offset to what I measured, 0.4041 and it didn't make any difference same action in SC. Tried several posts. The part shows up properly with lead-ins, rapids etc but when I run it, the torch ignores everything and runs off the table... Ideas?

Mike

[I Lean]

Use the MP1000-THC post, edit your switch offset like you've already done, and see if that changes things.

[Oldsarge]

I'll load it up at lunch today.... Hey, sorry I never got back to you on the measurements on those arms, do you still need them?

Mike

[I Lean]

Nah, I already made my bender. Thanks anyway!

As long as we're hijacking:

[Oldsarge]

Nice bender! Can't wait to use mine in some upcoming projects. Well, I ran over to the shop and I input the correct post processor..... Still the same problem, when I load any file it displays the tool paths etc but the gantry just flies off the display. Need to dig in the books I guess! Hope it's something simple like a setting or a checkbox somewhere!

[Oldsarge]

So I went to the shop after work today, and tried a few more things, watched the Sheetcam tutorials, and still can't seem to get any different results. I think I may delete Sheetcam and reinstall.... There were a few times I exited the program and it told me Sheetcam encountered an internal error. No matter what I do any combination of settings, drawings, whatever, when I run the simulation the torch head starts at 0,0 and just goes off to the upper right to infinity.... The start, pierces, tool paths are all there originating from 0,0 I believe I have the correct post loaded & edited now, so I don't think Mach is the problem. In sheetcam where the torch head goes from 0,0 to the upper right, when I attempt to run the gcode in Mach, the actual torch head goes from the point I have zeroed to the upper left. I have the machine, working envelope and material set up exactly as shown in the tutorials....

Will stop by the CandCNC user group as well.... Any thoughts welcome!


Oldsarge

[SignTorch Vector Art]

can you post the dxf and tap files so we're all looking at the same thing?

meanwhile, here is a simple gcode sequence, it traverses to 0,0 then moves along a clockwise square through 4,4, there is no Z motion

it should rapid move to 0,0, then feed up to 0,4, then right to 4,4, then down to 4,0, then left back to 0,0

save this to a tap file and run it in mach to verify your machine origin and axis orientation

once that motion is correct and verified it's just a matter of getting sheetcam to do the same

Code: Select all

(a clockwise square from 0,0 to 4,4)
G0 X0 Y0
G1 X0 Y4
G1 X4 Y4
G1 X4 Y0
G1 X0 Y0

[Oldsarge]

Thanks for that... Brilliant! A whole lot of marbles fell in the right holes just by running that file. I don't have internet at the shop yet so it's difficult to get the g code posted from here, but when I load & run a file with the torch off now, the file seems to be running except the z doesn't seem to be triggering at 0 or some offset when running... The z comes down & about lifts the gantry up. Also, it seems like when the gantry is moving during rapids that the torch head would be at or below the level of the plate, so either my z settings are wrong in Mach, or sheetcam isn't working with touch & go somehow? Getting closer though... Also, my torch was firing with clicking the icon before, but now I'm getting an overvoltage error now... Wth?


Oldsarge

[SignTorch Vector Art]

ok, next step is to test the Z direction

zero the Z somewhere up off the table

then you can type the gcode instructions into mach, or put them in a tap file

lines enclosed in parenthesis are comments, so you don't type those in, but they can be in a tap file

(lift torch 1 inch)
G1 Z1
(drop 2 inches to -1 inch)
G1 Z-1

if that moves in the right direction, that's good

when it's time to start a cut, sheetcam drives the torch downward (how far I don't know, but there should be a setting to limit the minimum Z to stop short of the table bed, either in mach or sheetcam)

during that move, the THC (or separate contact sensor) watches for contact, upon contact, the THC triggers mach to stop driving downward,

if a sensor never stops the down motion, mach will try to complete the down motion to whatever Z level it was instructed to move to (by sheetcam)

once it gets there, without contact sensing that would be the pierce height, with sensing that would be working zero and the Z would then raise to pierce height

after that it fires the torch and pauses (possibly waits for an arc start signal), drops to cut height, then starts the X-Y motion and engages the THC to monitor arc voltage

without a torch, you're missing the material sensing and arc start signal, so the pierce height and arc delay depends entirely on the gcode from sheetcam, so a viable pierce height, delay, and cut height must be set in sheetcam

[Oldsarge]

Awesome! More progress! I finally got what I think is everything (mostly) talking together. I had an issue with the air solenoid in the 1250 that I figured out and changed a few settings. I cut this Army seal, and the torch seemed to be firing from way up off the plate, and after it lit, it just sat there noticeably for several seconds before it started to move. Also, from the terrible cut you can see that most of it didn't cut... I think the Z was way high off the plate, and the torch sparked noticeably, but didn't light. Also, a few times I think I saw the torch rising as the cut progressed.

The cut is terrible, but it's proof that the thing works! I went back into motor tuning and noticed that the acceleration for each axis was very low, like 20 ipm. I have to spend more time in tuning obviously. Also in Mach on the setting screen, I have no option for steps... I had to go into the router profile, set & measure to get my steps per inch, then go into the regular profile, and enter the values in motor tuning. Is that right? Seems like I should be able to do that from the profile I run from...

Another question, when I use a tool in Sheetcam, I see that there is also cut profiles in Mach with a lot of the same information.... Should I be using both? Do they need to match, or does one cancel the other out? A little frustrated, but too excited to be discouraged!

Chasing out the gremlins! Here's some pictures of what I was able to get the table to do today....

Wavy wavy lines! I hope this is from the acceleration and motor tuning and not some physical problem like the gantry....

This looks like the pierces that the torch just sat there too long before moving....

Here you can see the areas where the torch was too high to get an arc ok, or rose off the plate and lost the arc. Every so many inches the z did come back down to the plate and reference itself, so that is promising.

Oldsarge

[tcaudle]

Did you go through the setup and tests in the DTHCII setup/Install Manual? Did you take note of the Torch Volts on a manual cut?

The first thing to do is do some simple shapes Lines, squares, circles and cut them with the THC button off in MACH and the Auto THC ON unchecked in the cut profile ALL of the motion prior to the DTHC taking over AFTER the pierce cycle and start of cut, are from G-CODE moves. If you can't make good cuts with the THC disabled it will not work with it on.
If the cut starts too high the voltage will be too high and the DTHCII Tip Saver will lock on. If you are failing to get penetrations either the gap is way too high or not enough current is flowing in the cut. The Workclamo should be ont he material and both ends clean ina tight for full current flow (think jumper cables here and what happens if you have a bad connection at either end)

It is important to adhere to the settings in the cut charts of your 1250. Using a nozzle that is too large (even if you crank the current setting down) will cause the voltage to skew up and the cut to be to wide. The THC will try to lower the voltage by moving the torch down. The cuts you show are no where close to being straight or correct.

It is important that you get a baseline of voltages from a cut with the THC tuned off. The values in the book are under the EXACT conditions listed (arc gap of .063, feedrate , correct nozzle, correct current setting, clean DRY air). for the material you are cutting. Change the conditions and the voltage will not be what the chart predicts. The PRESET VOLTS is a target voltage. It will not set absolute height (no matter what) it tries to move the torch in the direction the UP DOWN indicators show (at least it should) and tries to make the actual TORCH VOLTS natch the PRESET VOLTS.

If you are having problems with the base motion of your table than setup and do an "air Cut". turn off your plasma and use a POST (like MACH plasma ) that does not have a touch off sequence and watch the motion. Make some simple shapes like a 6" circle or a ^" square and watch them "cut" Watch the motion of your machine....is it smooth? Do the objects fall in the right place and does the motion follow the shape?

The first problem sounds like maybe a scaling problem where something is in mm and cutting in inches. Everything gets increased in size by a factor of 25.4!

Call the office and ask for some technical assistance. You will get someone that cuts with plasma and uses the software you have and knows the electronics front to back. Use the CandCNCSupport Yahoo Group. (2000 users with similar equipment)

I know you already know this but the new BladeRunner AIO User Manual off the website is a treasure trove of information about the basic machine setup and how to test all of the functions. tune the motors and check all of the inputs and outputs.

TOMcaudle

[Oldsarge]

Tom,

Thanks, I did go back to tge manual, and discovered if I read what's in there things start to work. Imagine that! I'm cutting now, and the thc is working great! The DRO displays the cut height, and I can see it minutely moving up & down during the cut. A few little things to dial in, but I'm getting it now. I'll be calling next week to ask about the motors, they get awefully hot, even if they are idle.... Other than that, I can't tell you how happy I am with the Dragon Cut!

Oldsarge