Z Diver Down

Hypertherm Plasma Cutter discussion forum.
Post Reply
Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 1:38 pm

New issue that I am hoping for some help with. I have been cutting a test file in 11 GA HRS which produces a small part about 3” x 5” with various shapes within (circles, squares, open lines, etc.). Initially, I was using the only nozzles that I had which were 65A, and I used the book settings altered between the 10 & 12 GA settings since there is no 11.

I cut the part 6 or 7 times while changing something in the tool set up each time such as IPMs, current, hole rules, well you get the idea. The results were just this side of awful. I ordered HT fine cut consumables and started going through the same process again. At 95 IPM, 45 amps and 78 volts it wasn’t cutting through completely but I could pop the pieces out. It left a lot of dross too on the underside, but when chipped off, looked really good. I eventually slowed down to 75 IPM and even bumped the Amps to 50 in order to try to get better results, but now I am in the weeds.

The torch touches off and fires, but in lieu of cutting the part, the Z continues down until the magnetic holder breaks away. I have tried numerous times with the same results. I have shut the system down including the pc, restarted and still the same results. When I try to run it with the torch disabled, it works but moves creepy slow through the file. I am stumped.

Thank you in advance.

Steve
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

User avatar
acourtjester
Elite Contributing Member
Elite Contributing Member
Posts: 3855
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z Diver Down

Post by acourtjester » Thu Jan 03, 2019 2:08 pm

When asking for help it would be nice if you give more info on you system, name of table (unless DIY but do say if it is) the software you are using if you are using THC, ohmic sensor, floating head switch. When getting lots of dross on the bottom is an indication of to slow movement of the torch. The movement of the torch into the metal at the start can be caused by a few things. In the g-code you need to have a cut height set to about 0.060" so after the pierce it know what height to stop going down at after the pierce. If you are using a THC having the voltage set to the correct arc voltage and a delay to wait until the arc voltage stabilizes about 1 to 1.5 seconds after the pierce (this is not the same as pierce delay).
It sounds like you have a Hypertherm PM65, my manual states mild steel 45 amps shielded (45 nozzle)about 133 volts and cut speed from 100 IPM (for 10 ga.) and 190 IMP ( for 12 ga.) . And I think fine cut nozzles should not be used on that thickness metal.
There should be no difference running the g-code with the torch on or off. If you have crashed nozzle into the metal you may have destroyed your shield and nozzle too that can really screw you up.
DIY 4X4 Plasma/Router Table
CandCNC DTHC-IV & Feather Touch
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PM 256 tig

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 454
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Z Diver Down

Post by robertspark » Thu Jan 03, 2019 2:35 pm

Mr. Fixit wrote:
Thu Jan 03, 2019 1:38 pm
The torch touches off and fires, but in lieu of cutting the part, the Z continues down until the magnetic holder breaks away
What is the thc doing? Sounds like the voltage sensed is too high (above the setpoint) and the torch is trying to move downwards to correct the voltage.

Do you have a pierce delay?

Do you have a thc delay after arcok set?

Post some code..... Give us a clue what software.... What thc.....
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 3:06 pm

acourtjester wrote:
Thu Jan 03, 2019 2:08 pm
When asking for help it would be nice if you give more info on you system, name of table (unless DIY but do say if it is) the software you are using if you are using THC, ohmic sensor, floating head switch. When getting lots of dross on the bottom is an indication of to slow movement of the torch. The movement of the torch into the metal at the start can be caused by a few things. In the g-code you need to have a cut height set to about 0.060" so after the pierce it know what height to stop going down at after the pierce. If you are using a THC having the voltage set to the correct arc voltage and a delay to wait until the arc voltage stabilizes about 1 to 1.5 seconds after the pierce (this is not the same as pierce delay).
It sounds like you have a Hypertherm PM65, my manual states mild steel 45 amps shielded (45 nozzle)about 133 volts and cut speed from 100 IPM (for 10 ga.) and 190 IMP ( for 12 ga.) . And I think fine cut nozzles should not be used on that thickness metal.
There should be no difference running the g-code with the torch on or off. If you have crashed nozzle into the metal you may have destroyed your shield and nozzle too that can really screw you up.
Ok, sorry for the lack of info. The table is a home built 4' x 4' running CandCNC Blade Runner, PM 65, Floating Head Switch and no Ohmic. The initial pierce is .150 and the cut is .060. I don't have any 220941 nozzles, using 220930 fine cut that I just got figuring that they would do a better job.

The THC does have a delay set to 1 sec in the code set through Sheetcam. The manual states 95 IPM @ 78 volts for 10GA. As I had mentioned, the cut was not complete at these settings so I have tried to slow down and also tried to raise the preset amps to 50. I will check things over again and look at the consumables as suggested.

Thanks..
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 3:14 pm

robertspark wrote:
Thu Jan 03, 2019 2:35 pm
Mr. Fixit wrote:
Thu Jan 03, 2019 1:38 pm
The torch touches off and fires, but in lieu of cutting the part, the Z continues down until the magnetic holder breaks away
What is the thc doing? Sounds like the voltage sensed is too high (above the setpoint) and the torch is trying to move downwards to correct the voltage.

Do you have a pierce delay?

Do you have a thc delay after arcok set?

Post some code..... Give us a clue what software.... What thc.....
Here is the code.

Thank you for looking.

Steve

You do not have access to view or download this file.
Become a Contributing Member to gain access to this feature. Click Here

4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

User avatar
acourtjester
Elite Contributing Member
Elite Contributing Member
Posts: 3855
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z Diver Down

Post by acourtjester » Thu Jan 03, 2019 4:28 pm

Well I see a few things that are not right and I think you should be running higher air pressure then 75 PSI, I think 85 PSI is the inlet pressure to the back of the unit.
The speed is way off during cutting, I see one at F3.937 for a ccw movement and another at 2.9527
DIY 4X4 Plasma/Router Table
CandCNC DTHC-IV & Feather Touch
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PM 256 tig

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 5:16 pm

acourtjester wrote:
Thu Jan 03, 2019 4:28 pm
Well I see a few things that are not right and I think you should be running higher air pressure then 75 PSI, I think 85 PSI is the inlet pressure to the back of the unit.
The speed is way off during cutting, I see one at F3.937 for a ccw movement and another at 2.9527
The pressure to the back of the unit is 110 psi. The feed rate is set to 90ipm in the tool table. I do see now that the number that you referenced of 3.937 shows up in Sheetcam on the "basic" tool tab for jet cutting which has always been there on all jet tools. Maybe that is what is being used for the torch off run as seen in the attached. I spoke with the tech support folks at CandCNC and although they had some suggestions, nothing resolved the diving issue.

link.https://www.dropbox.com/s/wht7p5ub2eo4x ... V.mp4?dl=0
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 5:52 pm

acourtjester wrote:
Thu Jan 03, 2019 4:28 pm
Well I see a few things that are not right and I think you should be running higher air pressure then 75 PSI, I think 85 PSI is the inlet pressure to the back of the unit.
The speed is way off during cutting, I see one at F3.937 for a ccw movement and another at 2.9527
The pressure to the back of the unit is 110 psi. The feed rate is set to 90ipm in the tool table. I do see now that the number that you referenced of 3.937 shows up in Sheetcam on the "basic" tool tab for jet cutting which has always been there on all jet tools. Maybe that is what is being used for the torch off run as seen in the attached. I spoke with the tech support folks at CandCNC and although they had some suggestions, nothing resolved the diving issue.

link.https://www.dropbox.com/s/wht7p5ub2eo4x ... V.mp4?dl=0
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

User avatar
acourtjester
Elite Contributing Member
Elite Contributing Member
Posts: 3855
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z Diver Down

Post by acourtjester » Thu Jan 03, 2019 8:23 pm

This is where I set each of the tool speeds in sheetcam, you may need to edit all your tool settings.
feed.JPG

You do not have access to view or download this file.
Become a Contributing Member to gain access to this feature. Click Here

DIY 4X4 Plasma/Router Table
CandCNC DTHC-IV & Feather Touch
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PM 256 tig

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Thu Jan 03, 2019 8:36 pm

That is exactly how I have it too. When I do a plasma set up in sheet cam, I select my file on the import menu, go to the operation tab then select plasma cut and I get the same screen. I select the tool from the drop down (which has all of the parameters) and go from there. This is the way I have done it for years with my prior TD machine without issue so I am confused. Thanks for the continued suggestions and help.
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

User avatar
acourtjester
Elite Contributing Member
Elite Contributing Member
Posts: 3855
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z Diver Down

Post by acourtjester » Thu Jan 03, 2019 10:41 pm

Ok I built 2 tables and used CandCNC DTHC-IV electronics and their SheetCam post processor which produce a different looking G-code. I am having trouble with some of the commands used with yours. I would reload both SheetCam and the post processor. It seems odd that changing the plasma unit would cause this kind of problem. The post processor is written for the electronics it is working with to communicate commands for table operations. You may need to find another member with a similar electronics and post processor, to find out were the problem is.
DIY 4X4 Plasma/Router Table
CandCNC DTHC-IV & Feather Touch
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PM 256 tig

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 454
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Z Diver Down

Post by robertspark » Fri Jan 04, 2019 4:40 am

In sheetcam

Is the machine setup as inches or milimeters?

In sheetcam, go to Options >> Application Options and review the Display + Units tabs.
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Fri Jan 04, 2019 5:33 am

acourtjester wrote:
Thu Jan 03, 2019 10:41 pm
Ok I built 2 tables and used CandCNC DTHC-IV electronics and their SheetCam post processor which produce a different looking G-code. I am having trouble with some of the commands used with yours. I would reload both SheetCam and the post processor. It seems odd that changing the plasma unit would cause this kind of problem. The post processor is written for the electronics it is working with to communicate commands for table operations. You may need to find another member with a similar electronics and post processor, to find out were the problem is.
Thank you for the suggestions. I will keep working on it and get back when I find the bugger.
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Fri Jan 04, 2019 5:36 am

robertspark wrote:
Fri Jan 04, 2019 4:40 am
In sheetcam

Is the machine setup as inches or milimeters?

In sheetcam, go to Options >> Application Options and review the Display + Units tabs.
I checked as you have suggested and found that the settings are in inches as I want them to be.

I also posted a note and the couple of attachments on the SC forum. Hoping to hear something from Les Newell

Thank you..
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

robertspark
Elite Contributing Member
Elite Contributing Member
Posts: 454
Joined: Mon Jun 12, 2017 6:43 pm
Location: nr Liverpool, UK

Re: Z Diver Down

Post by robertspark » Fri Jan 04, 2019 10:07 am

minor suggestion:

Post processor: CandCNCPlasmaLLCNC-rev16.scpost

May want to consider version 24D here:
https://www.candcnc.net/downloads/

I asked about inches because if you look at this GCODE

G38.2 Z-0.50 F#<_hal[gscreen.toffrate-s]> (Probe Touch-Off)
#<offset> = [#<_z> - #5063] (Find distance past probe touch)
G92 Z[#<_ini[AXIS_2]HOME_OFFSET> + #<offset>] (Switch Offset)
G1 X1.901 Y1.321
G0 Z0.150
M3 S100
G4 P0.5
G1 Z0.060 F150.0
F90.0
M67 E0 Q20 (DTHC is on)
G3 X1.965 Y1.257 I0.064 J0.000 F3.937
M67 E0 Q10 (DTHC OFF)
I0.000 J0.238 F2.9527
X2.029 Y1.321 I0.000 J0.064
G0 X2.030 Y1.322 (Add tiny extension)
M5
o<endcut> call

you will see that there is a number of feedrates which are well below F90 for arc motion
UCCNC,
Sheetcam
Hypertherm Powermax 45 (nonXP)
Neuron Lite THC
Hobby user (4x4 home table)

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Fri Jan 04, 2019 10:27 am

I will look into the update for sure.

Well, today is a new day and I gave the test another go. I am happy to report that we are back to snorkling and no longer not diving. however, disappointed because I have no explanation for the correct behavior. One thing that I did notice yesterday and although I have turned pages in the CandCNC bible, (without solution) is that the I/O 17 (P1 and pin 1) on the diagnostics tab was illuminated at at a steady state idle without cutting. Today it only came on at the beginning of the cut and went off. Not sure what that means.

As for the lower ipms in the code, I suspect that they relate to reduced travel speed which I have set in "path rules" in SC for small holes and shapes, but I could be wrong.

Also, and somewhat unrelated to the topic, I have had to significantly increase the amperage and feed rate from 45A to 55A and 90 ipm to 115ipm to get the best cuts with the 11Ga using the fine cut nozzle. Seems strange that book has values that are not even close for this.

Thank you,

Steve
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

User avatar
acourtjester
Elite Contributing Member
Elite Contributing Member
Posts: 3855
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z Diver Down

Post by acourtjester » Fri Jan 04, 2019 2:44 pm

The fine cut nozzle is rated at 45 amps and should not be used above that without much shorter life. I would buy some 45 amp nozzles in place of the fine cut nozzles for cutting 11 ga.
I have found that the path rules can be included in a g-code generation even when you turn them off in the tools section. if you don't want them you need to go to the tool menu at the top and go to path rules menu and under "Always apply rule set" to none.
DIY 4X4 Plasma/Router Table
CandCNC DTHC-IV & Feather Touch
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PM 256 tig

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Sat Jan 05, 2019 7:33 am

acourtjester wrote:
Fri Jan 04, 2019 2:44 pm
The fine cut nozzle is rated at 45 amps and should not be used above that without much shorter life. I would buy some 45 amp nozzles in place of the fine cut nozzles for cutting 11 ga.
I have found that the path rules can be included in a g-code generation even when you turn them off in the tools section. if you don't want them you need to go to the tool menu at the top and go to path rules menu and under "Always apply rule set" to none.
I understand the nozzle rating, just got impatient since I don't yet have the standard 45A nozzles. I did order a bunch of them and will have them early next week.

Interesting comment about the path rules. I will have to check that next time.

Thanks as always.

Steve
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

jimcolt
Elite Contributing Member
Elite Contributing Member
Posts: 3032
Joined: Mon Jul 20, 2009 11:18 pm
Location: New Hampshire

Re: Z Diver Down

Post by jimcolt » Mon Jan 07, 2019 3:52 pm

Trust me....the book specs are right assuming you are setting them exactly....and even more important, that the specs are being achieved. A few things to remember with plasma cutting of steel:

- if you are getting a drossy cut....do not slow down. Dross is most often caused by cutting too slow, cutting with the torch physically too high off the material, worn consumables or incorrect cut air pressure (different than the inlet pressure.
- Never cut at higher amperage than a nozzle is rated for. The best cut is exactly at it rating. If you run lower than a nozzle's rated amperage you get less arc energy density...and an ugly cut.
- With a new machine...especially homebuilt, ensure first that the cut speed that occurs during a cut (not what you set) is correct. Program a long straight line and do the math for the speed you set and time it to see if the speed is correct. For a newbie...there are a few things in machine code that will change the speed regardless of what you set!
- Install a pressure gauge hard plumbed on the inlet fitting of the plasma. If you do not have a gauge mounted here...then you do not know the dynamic (flowing) inlet pressure. Once the gauge is on...observe it with no air flowing to the torch. Then activate air flow, observe that the pressure will now be lower, the change in pressure is the pressure drop through your air plumbing system. Maximum static pressure at the inlet is 135 psi with a Hypertherm, minimum dynamic (flowing) pressure is 90 psi. Ideally, with flow you should be in the 100 to 115 psi range for most consistent results.
- Be sure you have the plasma set in aut gas mode...this ensures the cut air pressure (different from inlet pressure) is set for the torch lead length, the amperage, the consumables and the mode switch setting.
-Mode switch must be in continuous cut mode for cutting normal metal. If it is in gouge or expanded metal mode the cut pressure, the pilot current will be different, affecting cut quality rather dramatically.
- Make sure the consumables match those at the top of the cut chart for the material and amperage you wish to cut. The lowest amperage consumables should always be used for the material thickness you plane to cut if you want the best looking cut.Make sure the consumables...especially nozzle and shield are in good condition. Your manual has a page called "consumable inspection" that will help you!
- For your first cut I suggest doing the following: program a 1" wide x 3.5" long simple rectangle with a small radius on the corners and a 1/4" lead in, no lead out, one of the simplest parts you can cut. Put some 10 gauge steel on the table. Put a brand new set of Finecut consumables in the torch and use the 220948 shield. Set the torch to work distance with a .06" (16 gauge steel will work) thickness gauge. Jog the torch around and ensure it stays at .06" everywhere you will cut. Be sure to shut off the height control, do not allow initial height or pierce height....we need to stay at the cut height of .06" for this test. set the cut speed at 95 inches per minute. set the amperage at 45 amps. set pierce delay time at .5 seconds. Cut the part. I bet, assuming that you were getting 95 ipm out of your machine, that this cut is very nice. That is book specs. If the first cut has minor dross...do a few more cuts, each with a 3 IPM INCREASE in cut speed. At some point the dross...if it was there on the first cut....will be gone. Once you get to that dross free speed zone....observe your height control readout whil the cut is on the 3.5" straights on your rectangle. That is the arc voltage that you will need to set when everything is at book specs. It should be close (within a few volts) of the book voltage from the cut chart of 84 volts. If it is 10 volts high....then you will probably have to set all of your cut voltage 10 volts high in order to maintain the correct height. So set that voltage, activate the height control and do another cut. with height on, the book specs in, and the voltage set per your test...the cut should look the same with THC on. Let us know how that works! Jim Colt

Mr. Fixit
Posts: 61
Joined: Fri Aug 11, 2017 7:28 am

Re: Z Diver Down

Post by Mr. Fixit » Tue Jan 08, 2019 12:12 pm

Thank you for all if this great information.

Just for clarity, I did start with the book settings, but had to adjust for 11 ga since there was no infor that. At 45a with the speed between the 10 and 12 ga settings, I was not getting full penetration so that is why I slowed down.

The table is not new. It previously had another machine connected prior to the PM 65. I am awaiting the regular 45a nozzles and will go at it again

In the meanwhile, I cut some 5/16” HR with holes included and was amazed by the cut quality using 65amp nozzles and the machine set at 65a. The ipm was set at 60 and the rest was as per the manual.

I will continue to work on it.

Thanks again.
4' x 4' DIY Table
CandCNC Bladerunner
Hypertherm PM65 Machine Torch
Miller Vintage 250 Mig
Miller Syncro 180 Tig
Bridgeport 2J Mill - Fagor Dro
Southbend 14" x 40" EVS Lathe - Fagor Dro
Brook 18" Metal Shaper
Harig 612 Surface Grinder

Post Reply

Return to “Hypertherm Plasma Cutters”

Easyscriber engrave attachment for Hypertherm plasma cutters.