The Canadian Hack

[Mr.Hotwire]

The title says it all,

Im a soldier, an RCEME tech. I've taken NO REAL schooling in anything more the high school and some welding / fabrication night courses. But that hasn't stopped me. I have been building 3D printers, robots, and also obtained my Advanced Ham Radio License here in Canada. So, I guess I'm self taught in most of what I do.

I have been repairing welding machines, generators, and upgrading plasma cutters / tables as a side gig for about 3 years now. There are a few local shops that I have been doing this for, kind of like an "On Call" industrial maintenance man. Small shops of course, so its a bonus for both of us. I get some side money, experience and access to the shops, they don't pay for a regular employee to stand around. No one has complained.

I recently bought a bag of hammers, a CNC plasma table (4'X4') that the previous owner could not get to function. I mean.. there were a LOT of assumptions made in measurements and interoperability of parts, and non of those assumptions were correct. To the point where NEMA24 motors had mounting holes on 2 corners drilled out to fit onto NEMA23 Mounts. It was a mess.

After about 6 months of re-jigging and a LOT of parts replaced, I have a machine that is moving accurately, and should be ready for me to start making cuts. I have made some test cuts, but only of a testing nature to make sure that limits are being adhered to and that no MAJOR crashes are going on... I have crunched about $150 worth of limit switches, but that was purely my fault.

I have a MiniTHC installed, but not correctly setup. My Z Axis is also not correctly setup (or so I think). I need to figure out WHY my X axis is mirroring the directions of the DXF file, but jogs correctly with the MPG and MPI. SheetCam is the bane of my existence.. or at least getting a post that is compatible with my setup. This is a as much of a learning experience as I could make it, and I'm very happy about that. I ask a LOT of questions but that is what forums are for right? Plus if I find an error or solution, I feel its my responsibility to share that with everyone.

[robertspark]

I've been following your posts on the various forums.

I would suggest that you have something wrong with your setup, more than the miniTHC / sheetcam / uccnc being wrong.

Statements such as this one imply you need to stop and post more information on your setup.

I need to figure out WHY my X axis is mirroring the directions of the DXF file, but jogs correctly with the MPG and MPI. SheetCam is the bane of my existence.. or at least getting a post that is compatible with my setup.

Have you set up the axis the right way (the standard way)....
Press the left keyboard arrow and the machine jogs LEFT and the X axis numbers go DOWN (or get smaller or go negative)
Press the right keyboard arrow and the machine jogs RIGHT and the X axis numbers go UP (get larger or more positive)

Press the UP keyboard arrow and the tool jogs away from you and the Y axis numbers go UP (get larger or more positive)
Press the DOWN keyboard arrow and the tool jogs toward you and the Y axis numbers go DOWN (get smaller or go negative)

Press the PGUP keyboard button and the tool jogs upwards towards the ceiling from you and the Z axis numbers go UP (get larger or more positive)
Press the PGDN keyboard button and the tool jogs away from you and the Z axis numbers go DOWN (get smaller or go negative)

if any one of the above is not true, then you have an axis flipped and you will need to invert the axis direction setting in the software.

Don't try to fix too many things at once, first you need to get stuff moving the right way.

Sheetcam is VERY easy to use..... it's very simple and it exports gcode for uccnc and Mach3 which can all be used on UCCNC just fine.

The last thing to fix will be the THC once you get ALL of the other stuff done.

you DONT NEED THC its just a cherry on the top..... get the machine cutting in the right directions (outside cut clockwise, inside plasma cut anticlockwise).

Also do some linear parallel cuts (say 4" / 6" long) to find the optimum feedrate for your plasma cutter, like this
https://forum.langmuirsystems.com/t/lin ... t-file/569

Once you get some simple test parts out (say a 2" square with a 1" hole in the middle) you can now set up your cut offset to compensate for kerf width etc.

Holes (less than 1" dia) are normally cut at around 60% feedrate of the linear feedrate....... too quick and you will get a bevel..... too slow and you will get a lot of dross.

[jmersereau]

Hey Mr. Hotwire, I'm an Airman, RCAF AEC posted to Tyndall AFB FL, hometown is Fredericton, NB. I'm glad to hear that you are making progress and are able to keep your sense of humour and interest in learning.
I have been reading your various posts with questions and requests for help, I've tried to help you when I think I can add something or provide suggestions based on my past experiences. I would like to suggest that you close the loops with your various posts so that we and others who follow can learn from your adventure. Tell us what you have tried and what worked for you (and what didn't).
As suggested by Robertspark, working methodically, isolating variables and then changing one variable at a time will provide you with information of value and ultimately success.
Jim

[Mr.Hotwire]

Robertspark, I have done a full reinstall of Win10, removed all the bloat wear, and reinstalled UCCNC along with Sheetcam. Attached are screen captures of my UCCNC Settings (General, X/Y/Z&A Axis, IO and Spindle).

PGUP goes up, PGDN goes down.. all goes exactly the way you described above.

[robertspark]

1) your acceleration at 200mm/s/s is very low. you should be aiming for 0.3G (3000mm/s/s)..... basically see if you can bump it up a bit as it will help you to avoid rounded corners or loads of dross on inside corners.

2) how did you arrive at 200 steps per unit, what are you driving? what microsteps setting are you running, what is your math?

3) your linear error max and corner error max are VERY small at 0.03mm for a plasma cutter...... I would suggest trying 0.5mm ..... you could even go higher but try 0.5mm.... then bump it up to 1mm or 1.5mm and cut out some inside squares and see if you can accept the internal corner radii ...... it's a plasma cutter not a precision micro milling machine ..... a blunt chisel not a laser cutter.

4) spindle tab.... some of your thc control problems I suspect are from your M3 deyal on being set at 500msec..... basically it will fire the torch, wait half a second and do nothing before moving or starting the thc delay timer. set all of the delays to zero for delay on and delay off.

5) I will try to provide you with some simple test gcodes that you can dry cut. (see if you can fit a Sharpie to the plasma cutter with an elastic band and use a bit of paper to get the motion tested. to make sure X and Y are the right way


I will take another look and see if there is anything else that jumps out

[robertspark]

6) you have set your z axis with a homing input, but it seems to home in the negative direction AND you set the home coordinates as zero.

normally with plasma (and mill / router) you home at the top of the axis (positive direction) and you set the offset as your z axis travel 50mm or whatever.

because you have set your safe z as 25mm it will crash into your home switch as the top of the z axis if you were to use your safe Z position

you also have a probe input which I presume is the floating head switch input?

do you have an ohmic probe too?


I will come back to you with some other settings for the minithc when I get near my laptop for my old settings. (thc-lock and also the c-axis)

[Mr.Hotwire]

1/2) My acceleration was just the number that UCCNC had preset, I had lowered my velocity to 6500mm/min. A safe place to start, Im driving NEMA23's that are in turn driving 16mm ball screws. Above 6400mm/min velocity and Im skipping steps.

3) No excuse, I left it as it was from the setup. And my understanding of it was it is not going to impact my initial setup. So I wasn't worried about that yet.

4) My M3 Delay is because after the first cut is done, there is a delay between the M3 command and the actual firing of the arc, closer to 600ms. Should I be setting that in SheetCams pierce delay?

5) The Motion is correct now, for whatever reason doing the fresh install and setup corrected that error. It was PROBABLY a finger fault of mine that was corrected when I had to actually look at it. I am using SheetCam and the Mach3 Post, no THC at this time. I am cutting 50mm Donuts with 20mm center holes. See the attached video and image below.

6) I do NOT have a home switch on my Z Axis, I only have a floating head. The Ohmic Sensor is on its way, I ended up buying one rather than building one... I'm probably going to kick myself in the ass once I open it up to see exactly how its put together.

[Mr.Hotwire]

RS,

I tried your changed to the acceleration. with it set anything above 350 my cut quality was terrible. Also, I set the M3 delay to 0, and there was.. yet again.. the delay in the arc initiation.. so the cuts were missing the first 20-30 deg of the circles. this only happens after the 1st cut. There is NO delay on the first cuts

[adbuch]

The title says it all,

Im a soldier, an RCEME tech. I've taken NO REAL schooling in anything more the high school and some welding / fabrication night courses. But that hasn't stopped me. I have been building 3D printers, robots, and also obtained my Advanced Ham Radio License here in Canada. So, I guess I'm self taught in most of what I do.

I have been repairing welding machines, generators, and upgrading plasma cutters / tables as a side gig for about 3 years now. There are a few local shops that I have been doing this for, kind of like an "On Call" industrial maintenance man. Small shops of course, so its a bonus for both of us. I get some side money, experience and access to the shops, they don't pay for a regular employee to stand around. No one has complained.

I recently bought a bag of hammers, a CNC plasma table (4'X4') that the previous owner could not get to function. I mean.. there were a LOT of assumptions made in measurements and interoperability of parts, and non of those assumptions were correct. To the point where NEMA24 motors had mounting holes on 2 corners drilled out to fit onto NEMA23 Mounts. It was a mess.

After about 6 months of re-jigging and a LOT of parts replaced, I have a machine that is moving accurately, and should be ready for me to start making cuts. I have made some test cuts, but only of a testing nature to make sure that limits are being adhered to and that no MAJOR crashes are going on... I have crunched about $150 worth of limit switches, but that was purely my fault.

I have a MiniTHC installed, but not correctly setup. My Z Axis is also not correctly setup (or so I think). I need to figure out WHY my X axis is mirroring the directions of the DXF file, but jogs correctly with the MPG and MPI. SheetCam is the bane of my existence.. or at least getting a post that is compatible with my setup. This is a as much of a learning experience as I could make it, and I'm very happy about that. I ask a LOT of questions but that is what forums are for right? Plus if I find an error or solution, I feel its my responsibility to share that with everyone.

Thanks for sharing your story, and congratulations on your success with your various endeavors. It looks like you are getting some good information from the other members, but you might consider starting a new thread in one of the other categories such as CNC Plasma Cutters General Forum, DIY Plasma Table & Accessory Discussion Forum, or one of the others more appropriate to the discussion so that other members will more easily be able to share in the discussion and perhaps benefit from your experience with your table. Not too many (if any) will be searching the "Introduce yourself" section for ideas or information specific to this discussion.

David

[Mr.Hotwire]

Robert and Jim have been of GREAT VALUE. They have helped me, out of blue. I owe a LOT of my success to them, and other people who have reached out. I REALLY can't say that Iv received much better guidance anywhere.

I will move this over to another thread, thats also a great idea.

thanks again!

[robertspark]

RS,

I tried your changed to the acceleration. with it set anything above 350 my cut quality was terrible. Also, I set the M3 delay to 0, and there was.. yet again.. the delay in the arc initiation.. so the cuts were missing the first 20-30 deg of the circles. this only happens after the 1st cut. There is NO delay on the first cuts

turn the THC ON , this enables the ARC OK input.
also add pierce delay (G4 Pxxxx after the M3)

what material and thickness are you cutting?

what plasma cutter + amperage are you using?

the first pierce is always different to all other pierces. some add a pierce off to one side or in the waste as an initial start pierce

[Mr.Hotwire]

Im cutting 20g mild steel, I'm using a Primeweld Cut 60. I'm using 28a and 40 psi at 3600 mm/min. Pierce height is 3.6mm, cut is 1.5mm.

The post i am currently using is the Mach3 Plasma post. I have a copy of the post that was "written" for UCCNC with THC. My previous attempts were using the Mach3 THC and scriber.

I have gone over my Gcode, that was output by Sheet am, and there is nothing that was causing a delay on the M3 that would lead to the delay between torch on and the actual arc.

[robertspark]

I have gone over my Gcode, that was output by Sheet am, and there is nothing that was causing a delay on the M3 that would lead to the delay between torch on and the actual arc.

Can you post a bit / section of your gcode to have a look through.

___________________________________________________

You had (have?) a 500mSec delay that you added to your UCCNC M3 setup (M3 turn on delay) this will not help things.

Set that to ZERO and use a G4 Pxxxx affter your M3.

http://www.cncdrive.com/UCCNC/UCCNC_usersmanual.pdf
Also add M205 before your M3, this will enable THC and also enable the wait for ARC OK / Transfer signal.

As a TEMPORARY measure, add a M211 between M205 and M3 (this will disable / ignore the THC down / dive signal)

https://minithc.com/pub/MiniTHC2_EN.pdf
On the MiniTHC, set the THC Delay to 3 seconds (or maximum) (all this does it it does not provide an output for 3 seconds AFTER the Arc OK signal is recived. Again this is a temporary measure.

I am spinning plates at present and only have small amounts of time to try to help in snippets.

[robertspark]

Im cutting 20g mild steel, I'm using a Primeweld Cut 60. I'm using 28a and 40 psi at 3600 mm/min. Pierce height is 3.6mm, cut is 1.5mm.

Primeweld Cut 60 https://primeweld.com/products/cut-60-2 ... sma-cutter

SPECIFICATIONS:
BREAKER SIZE:
(120V) 30 amps
(240V) 50 amps
PLASMA OUTPUT IN AMPS:
Arc 120 volts: 20-30 amps
Arc 240 volts: 20-60 amps
DUTY CYCLE:
60 percent @ max rating (120/240V)
100 percent @ 23 amps (120V)
100 percent @ 46 amps (240V)
AIR PRESSURE:
40-75 PSI
AIRFLOW REQUIRED:
5 CFM @ 80 PSI

I cannot seem to find the correct owners manual as I'd like to see what it has within it (the link on the site is for a 160A stick + tig welder)

because of the amperage you are cutting at I would have said that the Hypertherm powermax 30 (or other similar amperage machines) would be in the same ball park for cutting speeds etc.

https://www.hypertherm.com/Download?fil ... &zip=False

Pdf page 72/98 provides a simple cutting table.... however the PMX 30 is not a cnc plasma cutter.... BUT, the same consumables are used in the PMX45 (non-xp) with the original (non-duramax) torch .... and that manual does provide some better machine cutting charts.

These will sort of probably get you in the right ball park given they are for a 30Amp plasma cutter / 30A consumables.

https://www.hypertherm.com/Download?fil ... &zip=False

If you look at pdf page 39-40 it will provide you with some initial settings for 30A cutting 20g (0.9mm) mild steel.
3.8mm pierce height, 1.5mm cutting height, 0 Sec (to maybe 200mSec) pierce delay [from TRANSFER / ARCOK signal!] at about 115V and 8100mm/min linear cutting speed.

if you decided to set the PMX45/30 at 23A instead.... 23/30 = approx 0.7666r therefore 0.766666 x linear feedrate (8100) should be in the same ball park 6210mm/min.

couple of caveats..... your plasma cutter has 60A consumables and you are trying to cut at 23A!.... the orifice in the middle is likely to be much larger than that required, turning down the amperage will probably make the arc a bit problematic and you may need to lower the cut height as the voltage will be higher trying to sustain the arc (probably! I am no expert in this. I use a PMX45 (non-xp) that has reams of cut charts and good cutting information.

The air pressure of the PMX 45 (and 30) should be around 90psi (6.2bar).... but they both have secondary regulators within them to reduce the cutting air pressure down to about 65psi (4.5bar) check you air pressure is not too high or too low and the arc is being extinguished / not being maintained. (try to do some hand cuts so you can demonstrate that the machine is not loosing its cutting arc and you have the right air pressure setup (the mange on the primeweld website is quite large...... 40-70psi......

here is a similar plasma cutter (it uses the same trafimet IPT 60 torch and has a 2x voltage setting of operation and it asks for 50psi when cutting at 120V (and 75psi at 220V input voltage) table on page 8/11

https://www.cncitalia.it/upload/cut%2055%20manual.pdf

The IPT60 is similar to the Trafirmet S60 (S65??) and that requires around 4Bar (58psi) of cutting pressure (at 60A), pdf page 42/400
https://shop.trafimet.com/en/files/ecom ... EA1102.pdf

unfortunately if your manual is not very comprehensive you are going to have to experiment a bit.

[jmersereau]

Here is the PrimeWeld Cut60 Chart...

Page30.jpg

Jim

[robertspark]

where did you find that?

(not quite legible as JPG for me).

[jmersereau]

where did you find that?

(not quite legible as JPG for me).

Hey, I scanned it from my paper manual, just rescanned at a higher res...

Jim

[robertspark]

nice. thanks, removes the guesswork

[jmersereau]

Here are a few more pages too, I started a new thread in...
viewtopic.php?f=4&t=32637
-
Jim

[Mr.Hotwire]

Here is my most recent .tap file for a simple donut. Im using the UCCNC w/ THC post from the Home Plasma Table Builders facebook page.

Code: Select all

N0010 (Filename: Donut (UCCNC MiniTHC Post).tap)
N0020 (Post processor: UCCNC MiniTHC.scpost)
N0030 (Date: 2021-07-17)
N0040 G21 (Units: Metric)
N0050 F1
N0060 G53 G90 G40
N0070 M206  (THC off)
N0080 (Part: New part)
N0090 (Operation: Outside Offset, Shape, T1: Mild Steel 20g, 30a, 40Psi)
N0100 G00 X85.6558 Y93.7167
N0110 G31 F50 Z-50
N0120 G92 Z0.0
N0130 G00 Z4.8000
N0140 G92 Z0.0
N0150 G00 Z2.5000
N0160 M213
N0170 M03 (Torch on)
N0180 G04 P0.6
N0190 G01 Z1.5000 F350.0
N0200 M205  (THC on)
N0210 G02 I17.2181 J17.2181 F3400.0
N0220 X84.3012 Y95.1873 I17.2181 J17.2181
N0230 M214
N0240 M05 (Torch off)
N0250 G00 Z10.0000
N0260 X75.8977 Y83.9586
N0270 G31 F50 Z-50
N0280 G92 Z0.0
N0290 G00 Z4.8000
N0300 G92 Z0.0
N0310 G00 Z2.5000
N0320 M213
N0330 M03 (Torch on)
N0340 G04 P0.6
N0350 G01 Z1.5000 F350.0
N0360 G03 I26.9761 J26.9761 F3400.0
N0370 X77.3483 Y82.5821 I26.9761 J26.9761
N0380 M214
N0390 M05 (Torch off)
N0400 G00 Z10.0000
N0410 X0.0000 Y0.0000
N0420 M05 M30

What I do notice is this "G04 P0.6". My SheetCam is setup to use MS as its time value, and my UCCNC is also setup to use MS as its time value. But SheetCam is sending it as P0.6, rather than P600.

UCCNC Time.PNG

SheetCam Time.PNG

[Mr.Hotwire]

BTW: I am using an IPTM-80 torch, with consumables for 30-40a (.09 oriface)

[djreiswig]

Are you entering 600 for the delay value in SheetCam? If you're entering .6 to then it's outputting that as .6 ms not converting it. I think the posts just output the delay value you enter.

[Mr.Hotwire]

Im putting it in as 600.

Tool 1.PNG

[djreiswig]

Search the post for G04 and see what code is after it. I'm not sure if it is some how scaling the number, or maybe it is a bug in SheetCam. I'm not sure how many people use ms.

[robertspark]

just change it to all (sheetcam + uccnc) work in seconds

600mS / 0.6S ....or 50mSec / 0.05Sec will make no difference in uccnc as the motion controller will add the correct amount of delay if it's in the right units.