Partial cut after pierce

[BrayD]

I’m having an odd issue. Machine pierces fine and the majority of the cut is as good as expected, but 1-2” after the piece is uncut.

Spectrum 2050 with 55a shielded consumables, running 55a and the recommended 70psi. 150ipm with a ramp rate of 4000steps/s^2. 0.150 pierce, .060 cut height. Cutting 10ga cold rolled sheet.

On parts like this I’ll simply slice it with a cutoff wheel and get on with my day.

This one left the entire line uncut though, which posed more of an issue. I had to re-cut these with a dremel.

I’ve studied the transition between pierce and cut height. Everything seems smooth and predictable. No idea why it’s failing to cut after the piece.

I’ve slowed to 130ipm which improves this a bit, but creates more dross. 150+ seems to be the ticket for clean cuts, I just need to figure this issue out.

[djreiswig]

Too short of pierce delay?
Incorrect cut height? Have you actually stopped and measured your cut height to verify it's correct?
Do you have your work clamp attached to the material and not just the table?

[BrayD]

Everything has been measured with feeler gauges. Ground clamp attached to clean material.

Pierce delay is very important with my setup. The torch will fire, pause (pause time is unspecified in my software), then drop to cut height. The time it takes before it actually moves is my pierce delay setting. I can set it so short that it moves before the torch drop.

If my delay is too long, it’ll drop to cut height, stay in one place, then dive when the THC takes over as the kerf is huge and so is the voltage.

If my delay is too short, it’ll move before the initial drop to cut height. This indeed results in a poor start-of-cut.

Right now it pierces, drops to cut height, then moves quickly to the material before the THC starts reading voltage. Minimal torch adjustment occurs after the THC takes over which makes me think everything is pretty dialed.

Interesting note - the perpendicular lead in is cut clean. The issue occurs after the 90* turn. That said, it still did it on the straight line path (no lead in) so I’m not sure lead in settings are the culprit.

This is all on a Torchmate 2 table using Sheetcam, TM2 driver software, and the red display AVHC.

edit: I'm very green with this table so please correct me if anything I've said is incorrect. One thing I've struggled with is that the THC is essentially independent from the g code. There's no Z in my coding, but it still drops to the cut height I've specified in Sheetcam somehow. I confirmed by running it in manual mode. Also not sure how to control the time between pierce and torch drop. That would be handy to figure out for thicker material I imagine. Current pierce delay is 3.6s for what that's worth. Much longer than that and it'll dive before it moves. Low 3's and it starts moving the torch before the torch drops to cut height. I digress.

Also of note, I ran a number of 6" test lines before cutting any of these actual parts and it seemed to be cutting well. Once I moved to the actual parts, it's giving me this issue. Something has to be off/changing. Just trying to figure out what variable to target so I can play with it to try to fix this.

[weldguy]

That is very odd, almost as if the torch is traveling too quickly after the pierce then slows down to the correct cut speed. Not sure how this would be possible but thats what it looks like if all of your heights are correct. Can you see if the torch is moving faster during that portion of the cut? Can you see if the cut height is incorrect for that first inch or so, could be the THC drops the torch down during that inch or so and then it cuts correctly. Gotta be something simple.

[acourtjester]

Some things for you to understand about the start operations, you may already know these but just as a refresher.
There ae 2 delays in the start operation, first is the pierce delay. It needs t be just long enough to pierce the metal, to long and you get a big hole, to short and torch moves before piercing.
Torch speed can effect the pierce time to slow and again a big hole, to fast no pierce. This is set in SheetCam. These are triggered by the Arc Ok signal (some use a different name)
The THC delay is to allow the arc to stabilize after the pierce and start moving of the torch, if not correct the torch dives or rises.
Now it sounds like you may have a stand alone THC which is independent to the G-code and has another separate motor to move the torch and may have another travel speed, then the Z axis. You said you have no Z travel commands in your G-code how do you establish pierce height or rapid height?
Normally the THC only controls the cutting height while actual cutting.
If you have a Proma SD it still uses normal Z axis movement commands and the signals pass through the THC to the driver, then if cutting separate signals are created by the THC to the driver for height control.

[BrayD]

This is difficult as I still don't have my arms completely around the variables I can change and how to change them. The standalone THC operation is confusing. This is my setup (photo taken as I was getting everything operational). I have officially entered the year 2001!

The Torchmate box with the readout is my THC. I set pierce height with a trial and error process using the potentiometer knob on the front of that unit. Multiple touch-offs while checking height with a feeler and making micro adjustments to that pot until it's at the height I want. Once it's set, it shouldn't change.

Cut height is set in Sheetcam. I set that height and run a test cut with the THC in manual mode (no THC control). Torch touches off, pierces, drops to cut height, then I lock that height by flipping it to manual and observe the constant voltage on the readout. To activate the THC for future cuts, I set it to auto and input the voltage I observed. The torch should maintain that cut height by monitoring voltage and adjusting cut height accordingly. I understand this unit is an antique and its performance is lacking at best.

I set rapid height in Sheetcam but haven't confirmed I'm achieving that in practice. Rapid height may be set in the THC and I have no control over it. Not sure.

I'm pretty sure the only delay I can control is the time to torch movement. This is set in the Torchmate driver software. I'm at 3.6s right now - that time is required to ensure the torch drops to cut height before moving. This is a snip from Torchmate - they recommend starting at 5s and modifying from there. I've found that anything over 4s causes torch dive.

Since you are using the height control unit to maintain the arc voltage during your cutting, you will want to start your M50 dwell at 5 seconds. This will allow enough time for the torch to lower to the material, sense it, back off to the Pierce Height, fire the pilot arc, penetrate the material and reach a stable voltage before the adjustment for voltage begins.

Link from where that came from: https://torchmate.com/avhc-help/Red-Display-AVHC

There's a chance that the first inch or so is when the torch is cutting at the Sheetcam cut height before the THC takes over. Even so, I don't see much Z movement if any at all when that occurs.

Assuming that's the case, I can play with the Sheetcam cut height to modify the height over that period. Given the uncut condition, would you guys say it's too close or too far from the material?

[acourtjester]

Old does not mean bad, You have a tool that will help you learn the operational fundamentals of CMC Plasma cutting. You may be able to update things as time and money allow. One of the things I see in the doc you attached to your post is what they call "Dwell Timing" they are incorporating what is call touch off into the total time for the operation. Where in a newer electronics the touch off completely separate and is not included in that time frame. The pierce delay does not start until after the Arc Ok signal is seen, in their 5 seconds time many things are happening. To give you an example steel 1/4" at 45 amps is like .6 seconds for pierce delay and then maybe about 1.5 seconds for the start of movement and arc stabilizing for the THC control. Maybe another member that is familiar with Torchmate software can give better help. One thing I would do is make sure you have a good air supply and maybe an pressure gauge at the input to the plasma unit to make sure the PSI does not drop to low at the start, and have about 120 PSI before cutting starts.
Here is their statement

Since you are using the height control unit to maintain the arc voltage during your cutting, you will want to start your M50 dwell at 5 seconds. This will allow enough time for the torch to lower to the material, sense it, back off to the Pierce Height, fire the pilot arc, penetrate the material and reach a stable voltage before the adjustment for voltage begins. The dwell time may need to be increased or decreased depending on the type of material, the thickness of the material, the program feed rate, and amount of amperage used. If you find that you are not getting the pierce quality you are looking for, it may be necessary to adjust your dwell timing. Start at 5 seconds, and then adjust the timing +/- 0.10 seconds depending on how the cut actually performs. Continue adjusting the dwell at .10 sec intervals until you achieve your desired pierce quality.

[BrayD]

Oh yes, fully agree with the equipment comment. I'm ecstatic that I have these capabilities in house. It's more than adequate for mechanical parts and I'm learning a lot getting it dialed in for more detailed work. I'll be a well educated consumer when the time comes to upgrade.

Also agree that the dwell time is accounting for a lot of operations. I wish I had control of each one independently, but I've been able to make it work thus far (less this issue I'm having here). I'm convinced that we can figure this out, even if cut quality suffers a bit in that first inch. Priority right now is getting it to cut all the way through.

My air supply should be pretty solid. I have 180 gallons of 100+psi supply. It wouldn't hurt to double check pressure at the machine though.
.

,
Back to weldguy's comment, I CAN set a max unramped speed as well as max ramped speed. I'm not sure how the machine interprets those inputs. Perhaps it's accelerating to the max unramped speed before my ramp rate takes over and controls the acceleration to the final cut speed. I would hope the unramped 'ramp rate' is similar to my applied ramp rate (otherwise I'd lose steps, right?), but maybe my applied ramp rate is conservative and there's indeed a difference in acceleration.

I may run some tests with my max unramped rate super low to ensure the whole acceleration is at the specified ramping rate.

Alternatively, I can play with my Sheetcam cut height as I think it'll be defering to that value for the duration of this cut length (1-2" before the THC takes over).

[acourtjester]

Not sure how you would find out but some of the older software were base on Mach3 with custom screens to hide that. Many of the software packages had motor controls built in, By this I mean you could adjust the acceleration and the velocity for each motor, this allowed you to dial in the best way to drive each axis. So you know there are 2 speed commands in the G-code to drive the axis motors. A G1 is controlled by the F number entered in the CAM software, that is how you set different speeds for cutting different thickness on material. A G0 is the fastest speed the motors are tuned for with the speed setting in the controller software. This allows for a cutting speed and a different rapid speed, for moving between cuts. Example the torch (Z) up/down would not be as fast the X and Y cutting action. Something to put in the back of your mind, you could change out the computer and the controller electronics. Retain the Drivers and motors and wiring. This would allow you to change the software to somethin newer and something you could get manuals that would be easier to learn and use. I have built a few tables so I could get experiences with different electronics and software. I bought refurb computers and tried different controller with their software. If you good with computers you may look into LinuxCNC as the software is free and the electronics is fairly priced, and the THC is much cheaper. Some are using the mini PCs, I went with a all in one type PC, something like this. but there are many others out there
https://discountcomputerdepot.com/speci ... s-10-home/

[weldguy]

If you decide to run some tests I would run it with the plasma off and you should be able to see and/or hear a difference in speeds if there is one. Let us know.

[BrayD]

My workflow is driving me to thinner material this week so I'm not sure I'll get any more test cuts in on the 10ga. Wanted to follow up here to keep this alive though.

I ran that same program with the torch off and didn't notice any speed anomalies (audibly or visually). Reading a few more posts about similar issues, people seem to think it's either the ground, air pressure, or torch height. Slowing the cut speed seems to cure it (as I've found as well), though that seems like a band-aid fix. I'd like to find the root cause. Many things to investigate when I get the time.

[djreiswig]

Could also be the material. I've had a steel sheet that gave me problems and then the next sheet cut great. Sometimes the composition is different.

[BrayD]

Cut height is set in Sheetcam. I set that height and run a test cut with the THC in manual mode (no THC control). Torch touches off, pierces, drops to cut height, then I lock that height by flipping it to manual and observe the constant voltage on the readout.

There's a chance that the first inch or so is when the torch is cutting at the Sheetcam cut height before the THC takes over. Even so, I don't see much Z movement if any at all when that occurs.

Assuming that's the case, I can play with the Sheetcam cut height to modify the height over that period. Given the uncut condition, would you guys say it's too close or too far from the material?

Replying with an edit as I did some more testing and found the above statements in bold to be FALSE.

Cut height is a setting in Sheetcam indeed, but my THC/control system does not use it. The drop to 'cut height' that I was referring to before is not driven by Sheetcam - it's the THC's voltage interpretation. I proved this by running a program in auto mode, but with the plasma turned off. It touched off on the material, backed off to pierce height, but never dropped to cut height. Any drop that occurs is due to the THC voltage interpretation.

I'm leaning towards this 10ga uncut phenomenon as being a torch height issue right now (as others have pointed out). I'll drop my pierce height to cut height and run in manual mode (no THC) to see what happens. If that solves the problem (at the risk of buggering up my consumables), I think I have my answer.

[BrayD]

I needed a couple 10ga tabs tonight so I cut them with no THC and pierced at cut height. 100% success.

Thanks to everyone for following this issue. I know it can be frustrating guiding someone who doesn’t know their equipment intimately. As I continue on this journey, I’m losing faith in my THC. I feel like it’s causing more harm than good at this point.
.

[acourtjester]

You can run tests on the THC to see how it behaves. Start a cut on a slopped section of metal with the highest part where you start. the THC should follow the downward slop, if it does not you will not damage your consumables. The torch will go out after a short time with no Arc OK signal, the same way it does if you go off the side of the metal.

[weldguy]

THC systems can be a pain when not functioning properly and/or not understood properly. I suspect your THC system is functioning properly or you would likely also be seeing cut height issues throughout the entire cut, not just the first little bit. I would continue to work with it in your spare time, I suspect it will be something very simple to get that pesky issue resolved. It seems to me that it is just too high off the material to cut through on that first couple inches, running some tests and keeping a close eye on it should uncover something.

[BrayD]

Appreciate the comments. I may continue to play with things as I do have a decent amount of this material on hand. For now I'm happy that I have a solution to get usable parts. Baby steps.