THC3T-02 voltage

[D3workz]

Hello plasma ppl!!!

Who ever has a THC3T-02 (from robot3T) I have this question... how do you obtain the voltage from the plasma?? I mean, is it the voltage with the torch cutting, or the torch free to air?

Technically, the latter does not make sense, as it would be the highest voltage and the area of control would be rendered redundant on the upper limit!

I have a torch free to air voltage of 270V and voltage whilst cutting 150V... (do I have something wrong here)...

But still, I wish someone that had success with this unit to clear this voltage issue for me... obvious that are other issues, but one at a time

Any help would really be appreciated here guys.

Thanks

Dim

[robertspark]

The voltage whilst cutting is the important voltage as this indicates the cutting height.

The voltage whilst in free air is arc stretch where the voltage is measured between the torch electrode and its internal (+) connection which is used for starting the arc. This voltage may have a lot of HF (high frequency) within it that your THC may filter out. Basically ignore this voltage.

Depending upon what plasma cutter you have they may provide cutting tables which indicate what 150v means ..... i.e. does it correspond to the cutting height at the cutting feedrate? Or is it too high? (150 tends to indicate being a bit high as the ranges I've seen are between 90-145V [from memory] but it depends upon the cutter you have .

[adbuch]

Hi Dim,
The arc voltage (or divided arc voltage) as measured while the torch is actually cutting is the proper voltage to use for your THC. This will allow your THC to monitor this arc voltage and adjust the cut height accordingly - in an effort to maintain a constant arc voltage and hence the correct cut height.
David

[D3workz]

The voltage whilst cutting is the important voltage as this indicates the cutting height.

The voltage whilst in free air is arc stretch where the voltage is measured between the torch electrode and its internal (+) connection which is used for starting the arc. This voltage may have a lot of HF (high frequency) within it that your THC may filter out. Basically ignore this voltage.

Depending upon what plasma cutter you have they may provide cutting tables which indicate what 150v means ..... i.e. does it correspond to the cutting height at the cutting feedrate? Or is it too high? (150 tends to indicate being a bit high as the ranges I've seen are between 90-145V [from memory] but it depends upon the cutter you have .

Thanks you clearing that. I have an Oxford 550 cutmaker unit, and for a single phase, its one heavy duty machine. I know you don't see these oxfords pop up in forums...but so far, its working like a gem.

[D3workz]

Hi Dim,
The arc voltage (or divided arc voltage) as measured while the torch is actually cutting is the proper voltage to use for your THC. This will allow your THC to monitor this arc voltage and adjust the cut height accordingly - in an effort to maintain a constant arc voltage and hence the correct cut height.
David

It is very clear and some what obvious now... but the manual of the THC (HAHA I am joking, it did not even come with a manual)....

What I ll do I ll level a piece of material, set the correct height that I want and monitor the voltage at that scenario. And I ll use that as the datum voltage for the THC.

One last question, would this datum voltage change if lets say I cut 4mm at 35amps and 10mm at 50amps mild steel with both having 1.5mm cutting height? Or do I need to create cutting scenarios to get the corresponding different voltages? (I know I can check this, but if I hear it hear it from you guys, I ll be more comfortable in knowing what I need to do.)

thanks

Dim

[adbuch]

Hi Dim,
The arc voltage is tied to both cut height, material type (steel, aluminum, etc) and current setting. So you will need to develop "cut charts" much like the ones provided by Hypertherm for their plasma cutters. So - yes - you will need to create cutting scenarios to get the corresponding different voltages for your particular machine.
David

[D3workz]

Great to know for sure. Thanks alot.

Dim

[adbuch]

Hi Dim,
I have attached a copy of the Hypertherm Powermax 65/85 cut charts so you can get some idea as to how the arc voltage changes as related to current setting and material being cut (for a given cut height). Obviously the values for your particular plasma cutter will differ from the Hypertherm values, but I think you can see the correlation between the different settings. Here is a sample page. You can click on the pdf attachment to see complete set of charts.
David

65A Shielded cut chart.jpg

Powermax65 85 cut charts.pdf

[robertspark]

I cannot find a manual for the Oxford 550 cutmaker

I did however find a 2 page pamphlet here: https://www.oxfordwelders.co.uk/plasma_10_510000238.pdf

which provides this table of cutting feedrates:

2020-08-08 10_08_41-250 _ 280 _ 300 _ 350 AMP MIG WELDING MACHINES.png

the feedrates for the hypertherm have no correlation to the Oxford 550 cutmaster. I suspect that this is because the cutmaster uses very low air pressure for their torches so removes less material as quick as the hypertherm powermax range.

2020-08-08 10_12_35-250 _ 280 _ 300 _ 350 AMP MIG WELDING MACHINES.png

I am not sure what amperage the 550's cut at but looking at the consumables it is probably 55Amps
https://migtigarc.co.uk/oxford-plasma-torch-185-c.asp

given it has a "rated output power" of 7.7kW / 55A would give a rated cutting voltage of 140V, which should be your starting point of target voltage (for 20/25mm plate), you'll find the target voltage will be lower at higher feedrates (or that is the way the hypertherm tables go)

[robertspark]

It is also probably worth checking that you have the RIGHT consumables for cnc plasma cutting with the Oxford 550 cutmaster too.

It appears to use the Trafimet S65 torch (which is a good torch from an italian torch manufacturer [thats all they do, make torches for plasma, mig & tig])

The consumables listed for that torch actually include / show the drag cutting attachment..... i.e. you don't want to be using it for cnc unless you ran say a sprung loaded Z-axis (which would negate the need for a THC )

https://www.tbws.co.uk/shop/trafimet-cv ... hment-s65/

The consumable part numbers are shown around page 28/30 of this PDF:
https://trafimet.com/catalogues/Trafime ... orches.pdf

[D3workz]

Hey guys, thank you so much for your help here!!!

To tell you the truth I had that oxford pamphlet but I did not give it much importance.

Regarding the torch, I am not using the S65, I have the S65P, which is a pen type torch for CNCs. I use both the 40Amp and 60Amp consumables, depending on what I am cutting. (link to torch S65P - http://www.onlineweld.com/autocut-pa221 ... aptor.html )

As for the floating Z, I ve been using a floating head with a probe switch. I used to just probe the top of the material once before I do my cut... or if I have many long cuts, I would probe randomly as I progress thru the sheet I am cutting (btw my table is a DIY table that I have built and has a bed size of 1.25m x 2.5m).

Now that I have "upgraded" with a THC, I am looking to edit the M3 macro to force the probe function before every M3 (i.e G31). I need it to work this way, since every time the THC makes a correction, Mach 3 would not know about it, and I ll lose the Z height.... or at least this is what I think I want hehe...

Just something about me, I am used to work with CNC mills/router, in fact I have one that I have built some time ago... but this plasma is a big adventure as I ve never used a plasma before, not even a hand held one.

Guys, once again I thank you for all the help.

Dim

[acourtjester]

forget it no post issued

[adbuch]

You're welcome Dim!
David

[robertspark]

Now that I have "upgraded" with a THC, I am looking to edit the M3 macro to force the probe function before every M3 (i.e G31). I need it to work this way, since every time the THC makes a correction, Mach 3 would not know about it, and I ll lose the Z height.... or at least this is what I think I want hehe...

Yes Mach3 will loose track of the zaxis position so it is probably best to touchoff before each pierce that way you know you are starting at the right cut height (this is normally done either in the post processor or via a macro which the post processor can call)

I'll presume that you are working in Metric

Code: Select all

G31 X-100 F500
G92 Z-xxxx (where xxxx is your switch offset)
G0 Zyyyyy (retract to pierce height)
M3 ( DoSpinCW() )

find the switch offset using the MDI and probing with:

Code: Select all

G31 Z-100 F500
G92 Z0

using a piece of paper jogging axis, upwards until the paper slides out and read the DRO value, that will be your negative switch offset value for the floating head (use a thick piece of steel so it does not flex like say 2mm will with the weight of the torch on it, depending upon your bed support spacing)

[D3workz]

Now that I have "upgraded" with a THC, I am looking to edit the M3 macro to force the probe function before every M3 (i.e G31). I need it to work this way, since every time the THC makes a correction, Mach 3 would not know about it, and I ll lose the Z height.... or at least this is what I think I want hehe...

Yes Mach3 will loose track of the zaxis position so it is probably best to touchoff before each pierce that way you know you are starting at the right cut height (this is normally done either in the post processor or via a macro which the post processor can call)

I'll presume that you are working in Metric

Code: Select all

G31 X-100 F500
G92 Z-xxxx (where xxxx is your switch offset)
G0 Zyyyyy (retract to pierce height)
M3 ( DoSpinCW() )

find the switch offset using the MDI and probing with:

Code: Select all

G31 Z-100 F500
G92 Z0

using a piece of paper jogging axis, upwards until the paper slides out and read the DRO value, that will be your negative switch offset value for the floating head (use a thick piece of steel so it does not flex like say 2mm will with the weight of the torch on it, depending upon your bed support spacing)

I think I would like to edit the M3 marco just because I ll have control on the Z feed rate whilst processing the G31 (probing function).

All the post processors that I managed to find are limited in what you can edit whilst exporting from Fusion360... (I am very new to this, hence I dont know how to edit the post processor)... HOWEVER.. I THINK that if I edit the M3 like this (again this is all from extensive research these couple of days):

Code("G31 Z-50 F2000") {Here I can set the feed rate of the Z - yes I am a metric person}
While Ismoving()
Wend
Code("G92 Z0")
While Ismoving()
Wend
Code("G0 Z -12") {this is my probe switch offset}
While Ismoving()
Wend
Code("G92 Z0")
While Ismoving()
Wend
Code("G0 Z3.5") {typical pierce height}
While Ismoving()
Wend
DoSpinCW() {Turn on torch}

I can get away with running the probe function before each M3, and I can set the feedrate as fast as I want and avoid trying to find a good Post processor with what I need...but there again I might be mistaken and I ll end up here asking LOL....

Since we arrived here - can you decipher the above code, and explain to me if this will work or not?
BTW I am hopeless at coding.

Thank again Dim

[robertspark]

....

below is the edited VB Cypress macro code that should work for you.
G31 will move a set distance until it is triggered or it exceeds the set distance where it will throw an error, hence its good to put a big number here (bigger than the travel distance of your z-axis)..... the feedrate is quite high at 2000mm/min (33 mm/sec), the problem is technically where the z axis stops is not actually where the G31 skip signal was triggered...... because the axis will accelerate to a stop, hence if you were to do the movement exactly as it should be done.... you would add in the following line which will backup the z axis to the exact location that the skip signal was actually triggered (not where the axis decelerated to a stop)

Code: Select all

Code("G0 Z#2002") {moves back to the skip signal trigger point}

hence if you use a slower probing speed the deceleration distance will be smaller and the error could be ignored (given you calculated the offset from this error point).

its good practice to give mach3 a bit of a sleep between commands so that they register IMO (YMMV) [100mSec is neither here nor there...]

G92 sets a temporary offset it does not need a While ( IsMoving())

also keep an eye on the syntax [Ismoving is not the same as IsMoving]..... vb is more forgiving than c and that damn ";" colon!

Code: Select all

Code("G31 Z-100 F2000")  {Here I can set the feed rate of the Z - yes I am a metric person}
While ( IsMoving() )
sleep (100)
Wend

Code("G92 Z0-12")  {set negative probe switch offset}
sleep (100)

Code("G0 Z3.5") {typical pierce height}
While ( IsMoving() )
sleep (100)
Wend

DoSpinCW() {Turn on torch}

here are a couple of manuals for you:
https://www.machsupport.com/wp-content/ ... og_Ref.pdf
http://www.machsupport.com/wp-content/u ... mmands.pdf
https://www.machsupport.com/forum/index ... tach=18779

[D3workz]

....

below is the edited VB Cypress macro code that should work for you.
G31 will move a set distance until it is triggered or it exceeds the set distance where it will throw an error, hence its good to put a big number here (bigger than the travel distance of your z-axis)..... the feedrate is quite high at 2000mm/min (33 mm/sec), the problem is technically where the z axis stops is not actually where the G31 skip signal was triggered...... because the axis will accelerate to a stop, hence if you were to do the movement exactly as it should be done.... you would add in the following line which will backup the z axis to the exact location that the skip signal was actually triggered (not where the axis decelerated to a stop)

Code: Select all

Code("G0 Z#2002") {moves back to the skip signal trigger point}

hence if you use a slower probing speed the deceleration distance will be smaller and the error could be ignored (given you calculated the offset from this error point).

its good practice to give mach3 a bit of a sleep between commands so that they register IMO (YMMV) [100mSec is neither here nor there...]

G92 sets a temporary offset it does not need a While ( IsMoving())

also keep an eye on the syntax [Ismoving is not the same as IsMoving]..... vb is more forgiving than c and that damn ";" colon!

Code: Select all

Code("G31 Z-100 F2000")  {Here I can set the feed rate of the Z - yes I am a metric person}
While ( IsMoving() )
sleep (100)
Wend

Code("G92 Z0-12")  {set negative probe switch offset}
sleep (100)

Code("G0 Z3.5") {typical pierce height}
While ( IsMoving() )
sleep (100)
Wend

DoSpinCW() {Turn on torch}

here are a couple of manuals for you:
https://www.machsupport.com/wp-content/ ... og_Ref.pdf
http://www.machsupport.com/wp-content/u ... mmands.pdf
https://www.machsupport.com/forum/index ... tach=18779

Yes you are right... I need to compensate for the overshooting of the Z axis... Well what can I say.. I really appreciate all the help you have given me so far!

Tomorrow I ll try to find some time and go play with these macros, obviously I ll try your code and see from there... come what may, I ll let you know what happened.

Btw, thanks for the links... these shall be very helpful.

Regards

Dim

[robertspark]

no problem, here to help and learn too.

have fun

[Rodw]

I can confirm that you should never use the Hypertherm cut charts with any other machine. Its totally different.

Probably not helpful but I measured the THC3 divider as being

Code: Select all

21.2775:1  (measured 4.54v output on a 96.6v input)

With regard cut charts, 150 volts sounds high but in the ball park. The Traffimet 70 amp machine torch I had on my Everlast 50s should be similar

Try 3.5mm pierce height, 1.75mm cut height, 0.2 sec pierce delay

for Cut speed on 2mm mild steel try 2.0mm/min, Voltage will probably be about 90 volts but I might be way off.

I would ignore the voltage to start by cutting a series of 6 inch cuts at 1.75mm height with THC disabled say 10mm apart. Make your gcode cut them out so you can take them away to study them. start at 1800mm/min going up to 3000 mm/min in 100mm increments. Hit the stop button if it does not cut right through. Then pick the cleanest looking cut and repeat a series of cuts from -50mm/min to + 50mm/min from that. Picke the best again. Lets use that as your cut speed.

So now at that cut speed, repeat the exercise from 1.5mm to 2.5mm cut height in 0.1mm increments. Pick the best looking cut again.

You should be pretty well dialed in now. If your chosen cut height is too far away from 1.75mm redo the test process again.

If you've been observing the cut voltage through this process you should have a feel for it by now.

Make some final test cuts and observe the torch voltage. Allow 1.5 to 2.0 seconds for the torch to settle to its natural cut voltage and observe the torch voltage. Thats it you have it done for that material and thickness. That is the voltage you use. You can enable the THC now. I would work with a THC start delay of about 1.5 seconds to start with.

You can experiment with the pierce height but really thats to save your consumables. Once you have set your cut height, you can use that for every thickness of that material.

[adbuch]

The Hypertherm cut charts were shown for comparison only - to give some idea how the different settings change with amperage, voltage, cut speed, etc.
David

[adbuch]

As stated in the original response: " Obviously the values for your particular plasma cutter will differ from the Hypertherm values, but I think you can see the correlation between the different settings."
David

[D3workz]

As stated in the original response: " Obviously the values for your particular plasma cutter will differ from the Hypertherm values, but I think you can see the correlation between the different settings."
David

Hi David,

firstly thank you for your replies... I really appreciated!

Just to put it there, I wasn't comparing my Oxford with any of the hypertherm machines... I am sure that hypertherm are the rolls royce of plasma, HOWEVER, even though I never owned a hypertherm, I am very pleased with this Oxford machine. Its tough, never miss a beat and cuts like butter.

As regards to voltage (referring to the initial question of this tread), yesterday I cut some 20 mm mild steel at 200mm/min with out any problems... I did not experiment, hence I might have gone 250mm/min but anyways, the voltage on my THC was around 145V and was cutting at 50 Amps....

Maybe this will of some help to someone

Anyways, thanks guys

Dim