[multiplex]

hoping maybe jim & tom can chime in on this thread

so i'm getting the hang of my new machine, but have a few questions

i'm using a hypertherm 1000, with 60A tip and machine shield.

i've been cutting both 1/4" and 1/2" CRS, at 86 & 27 IPM respectively

for controls i'm using the bladerunner setup, with DTHC

questions

1. how much bevel should i expect on 1/4"? Is it possible to get none? 1/2" i'm getting about .025" bevel from top to bottom. But i'm also getting that with the 1/4"

2. mach is reading higher torch voltages than the setpoint. it appears to be making changes to the Z, but still not hitting the target. What do i check for? In the video below about 30 seconds in you can see my mach screen. some of my final cuts with the 1/2" the torch voltage was very high (170?) and the torch was high above the work.

3. i was cutting some 1/2" and when it got back around near my entry point, the torch would dive down and hit the metal - i'm assuming this is a setting in the DTHC. i seemed to have gotten it to work afterwords, but not sure what i did

guess thats all for now

[nomedia="http://www.youtube.com/watch?v=plpzPksGRqY"]YouTube- First Plasma Cuts[/nomedia]

[Mike 1948]

Just for my own education(I'm new at this), how do you get by without the ground clamp on the material for the cutter in video? Is it because you are using a water table and the clamp is on that? I tried cutting without a ground a couple of times(due to a brain fart) and the torch, a Cutmaster 52, would not cut well at all.

Just Curious
Mike

[multiplex]

mike - good question, and hopefully people can correct me if i'm wrong. I have the ground clamp on my water tray - figuring its connected through all of the slats, etc. Should it be directly on the piece?

[Mike 1948]

mike - good question, and hopefully people can correct me if i'm wrong. I have the ground clamp on my water tray - figuring its connected through all of the slats, etc. Should it be directly on the piece?

I am fairly sure you should have it directly on the work piece. I never had any luck without the clamp being directly on the work piece. I would give it a shot and maybe your issues will resolve themselves.

Mike

[jimcolt]

You can get bevel down to maybe 1 to 1.5 degrees on 1/4" steel with the correct setup with your air plasma. There are industrial high definition class plasmas (cost 10x more than your Powermax!) that will cut with close to 0 bevel.

1. Always use the lowest power option that is rated for the material thickness if you are desiring minimum bevel, best part accuracy. If you look at the mechanized cut charts (yes, use the mechanized consumables and mechanized cutting specs, even if you are using a hand torch on your machine) you will find that the 40 Amp consumable are specified for cutting 1/4".....the fine cut consumables are smaller, and lower power, but are only rated to 1/8". So put the 40 Amp consumables in, follow the optimum specs for speed.....and for best angularity subtract about 10 to 25% from the optimum listing...you may get some fine dross, but it will be very easy to scrape off...this is called low speed dross. So, I would cut at 40 Amps, torch to work distance exactly 1/16" (adjust arc voltage during the cut to achieve this physical height, don't wory about the voltage reading)...cut speed at about 40 ipm, pierce height of 3/16" (important, one pierce too close will damage the nozzle orifice, which causes bad angularity), pierce delay of 1 second. You can experiment by bumping the speed up a 5 ipm at a time, you may eliminate the dross and still get a respectable cut edge squareness.

2. The arc voltage is the actual measurment of voltage between the negative electrode inside the torch, and the plate, which is positive. When the plasma arc gets longer (electrode further from the plate) the voltage gets higher. The height control compares the preset arcvoltage to the actual, and adjusts the z axis until they are close to matching. There are some $15,000 industrial height controls that can hold the voltage matching to within .5 volts (equates to about .03"), however on an air plasma...if you can hold to plus or minus 5 volts your height should be ok. If the height control z axis is hunting or oscillating...then there likely is an adjustment (gain?) that Tom can help you with. As stated in number 1 above, the physical height (when using the machine shield on the torch) is the critical factor, if the voltage does not match the plasma manufacturers specs for arc voltage...ignore it...and adjust the voltage during steady state cutting until the physical height is correct. As the electrode in the torch wears, you will find you may have to run at 5 to 10 volts higher (near the end of the electrode life) than you would with a new electrode. Some of the $15,000 THC's automatically compensate for electrode wear by recalibrating at the beginning of every cut.

3. Think of how the torch height works, by measuring arc voltage. When the arc gets longer, the voltage gets higher, and the z axis moves the torch closer to the plate. If, at the end of the cut the torch crossed the kerf, the plasma arc gets longer to reach metal, and the height control will naturally move the torch toward the plate. There likely is a setting either in mach, or a height control adjustment that will remedy this issue...Tom likely can answer that.

Hopefully this helped a bit...good luck in your learning curve!

You should have your work clamp securely bolted to the slat bed on your machine. If you are cutting small pieces, or thin aluminum...you may want to fabricate a heavy gauge jumper wire with an alligator clip (rated for maximum current of your plasma) from the work cable connection directly to your plate.

Jim Colt

hoping maybe jim & tom can chime in on this thread

so i'm getting the hang of my new machine, but have a few questions

i'm using a hypertherm 1000, with 60A tip and machine shield.

i've been cutting both 1/4" and 1/2" CRS, at 86 & 27 IPM respectively

for controls i'm using the bladerunner setup, with DTHC

questions

1. how much bevel should i expect on 1/4"? Is it possible to get none? 1/2" i'm getting about .025" bevel from top to bottom. But i'm also getting that with the 1/4"

2. mach is reading higher torch voltages than the setpoint. it appears to be making changes to the Z, but still not hitting the target. What do i check for? In the video below about 30 seconds in you can see my mach screen. some of my final cuts with the 1/2" the torch voltage was very high (170?) and the torch was high above the work.

3. i was cutting some 1/2" and when it got back around near my entry point, the torch would dive down and hit the metal - i'm assuming this is a setting in the DTHC. i seemed to have gotten it to work afterwords, but not sure what i did

guess thats all for now

YouTube- First Plasma Cuts

[Torchhead]

Poor connection to the workpiece causes the voltage to not operate within the range on the chart. (takes more voltage to get the proper current density). ALWAYS clamp the workclamp to the material. If you don't hold the 1/16th recommended arc gap then your cut flair will increase and cut quality suffers. When the voltage climbs outside the percentage you have set on the Tip Saver (anti-dive) then it locks any DOWN movement. Once the voltage spirals out of the proper range it's hard to get it to adjust itself back. The DTHC will hold better than 1 V (it has a settable "Span" value from as low as 1/4 volts to several volts). of arc volts while cutting. The two most important indicators (besides torch volts) are UP and DOWN. Since the DTHC signals MACH to raise or lower the Z (similar to an external jog command) the signals displayed on the screen are important to analyze what is happening. If the UP is on the Z SHOULD be moving UP. Conversely if DOWN is on it should move down. If you are not getting a DOWN indicator if the voltage climbs above the Preset then either the TIP SAVER has cut in or the communications between MACH and the DTHC are not working. The DTHC has a self test that will let you quickly confirm you have all the proper signals.

If you setup and cut a line with the tip at .063 above the material and at the recommended optimum feedrate with the THC Button OFF in MACH you can observe what the DTHC is doing. The voltage should be close to the chart voltage for that material and nozzle. If it is not then you have physical problems with the plasma. The voltage is your "altitude" reading. If it's off then so will be your cut. As it cuts manually observe the Torch Volts reading; it will change but if the material is flat and the cut is a straight line it should not change more than a few volts.

The other common mistake I see a lot is the THC Corrections (settings tab) gets "adjusted". The numbers are the absolute Z values it will allow (Max and Min) as it cuts. They are defaulted to +1 and -1. If you are running in INCHES units then that basically turns it off. If you happen to be using MM it prevents any movement at all. Set both to 0 and you get no adjustment at all. Set the MIN to high and it will just ratchet up the torch evn though the poor DTHC is screaming "MOVE DOWN, MOVE DOWN"

The last thing is about Grounding. The table needs to have a solid earth ground (ground rod). The workclamp out of a plasma is not ground and does not ground the table. If the table is floating then it can be a hundred volts above a true earth ground. Grounding the table is not only for safety but to keep the nasty noise off the table structure and from being transmitted back down wires to the control electronics.

We got to great lengths to keep the low voltage control signals totally isolated from the noisy plasma. If the noise is enough to be inductively coupled across or radiated through the air it defeats the isolation we designed in.

TOM caudle
www.CandCNC.com

[multiplex]

been reading and re-reading alot of these posts, plus being doing a bunch of practice. Things are starting to come together! thanks everyone for the help.

i do have one new question though

tonight i was doing some 3/8" steel. 60amp tip. about 41ipm.

when doing a straight cut, the voltage is a perfect 141. I verified this by turning off THC, setting cut height and making a straight cut.

I then cut some profiles using the THC, and again things were great.

I then cut some small holes (about .4" diameter). and the torch wants to dive hard into the plate. I turned off THC and set cut height to .0625, the voltage that it reads is 151 or above. The hole looks good, but i'm just wondering why the voltage would be higher?

I then go back and do a straight cut, and its back to 141

I have the ground directly on the stock.

Any thoughts? I'm thinking about just cutting these holes without THC. is there a way to turn it off mid program?

[jimcolt]

When you cut small holes or fine features with plasma cnc machines...because of the small features of the hole your machine is not acheiving the programmed cut speed. In your example, the true contouring speed of the torch on the small holes is probably much less than the 41 inches per minute that it is travelling at on the straight sections of your cut....this speed reduction is simply because the machine cannot make the tight corners and accelerate to full speed in such a small area. This is typical with the vast majority of cnc plasma machines...and even more so when using a plasma with higher speed capability.

On most Industrial cnc controllers (Hypertherm and Burny cnc) there is a prameter setting in the background setup files that compares the cut program speed to the actual speed that the machine is able to achieve, and this is measured through the drive feedback loop (encoder feedback on servomotor drives). This parameter is called something like "height freeze" or "corner lockout" depending on the machine manufacturer, and it often is set at 80%, which means whenever the true contour speed drops below 80% of the program speed (or operator set speed) then the cnc sends a signal to the z axis that freezes the height at that moment, which eliminates the torch dive during slowdowns. This generally occurs during small holes, fine features and even during de-acceleration and acceleration going in and out of corners.

Why does the THC dive? The arc voltage feedback THC is essentially a comparator circuit....it compares the operator setting (in your example 141 volts) to the actual arc voltage as measured from the negative electrode to the positive plate. If the actual voltage is lower than the operator set voltage, then a signal is sent to the z axis drive to raise the torch until the two voltages are the same. Consequently if the actual voltage reading is higher than the set voltage, the z axis moves the torch closer to the plate to make both voltages equal.

The arc voltage is a stable method of monitoring torch height, but only at a fixed cut speed. When the machine slows down, the plasma arc continues cutting at a fixed power level, this causes the arc voltage at the torch to increase as it is burning a bit of a wider kerf....so when the voltage increases on a speed slowdown, the THC adjusts the actual voltage by moving the torch closer to the plate. When the slowdown is substantial, the torch can actually hit the plate. There needs to be a height freeze in these situations, and I'm sure there is a setting in your system, and I'm sure Torchead can help with it, that has the ability to eliminate diving in corners and on small features.

Another point or two.....don't dwell on the voltage setting, consider it simply a reference on air plasma systems. It is most important to maintain the plasma torch manufacturers physical torch to work distance while cutting. If the cut charts (such as the ones in a Hypertherm manual) list a voltage, use that as a starting point only (should be in the ballpark!) but adjust your voltage up or down to ensure that the physical standoff is exactly correct, this will provide the best cut. As the torch electrode develops a pit during normal wear, the arc length will get longer. It is absoltely normal to have to run 5, 10, or 15 volts higher with used consumables in the plasma as compared to new ones....in order to maintain the important torch to work distance.

On high end (read expensive) industrial high definition class plasma systems the arc voltage is built into the part program automatically, and some of the better torch height controls calibrate the voltage/physical height ratio at the beginning of every cut cycle to compensate for electrode wear and to automate the process. Just the height control system for these industrial machines can be $15k.

Jim Colt Hypertherm

been reading and re-reading alot of these posts, plus being doing a bunch of practice. Things are starting to come together! thanks everyone for the help.

i do have one new question though

tonight i was doing some 3/8" steel. 60amp tip. about 41ipm.

when doing a straight cut, the voltage is a perfect 141. I verified this by turning off THC, setting cut height and making a straight cut.

I then cut some profiles using the THC, and again things were great.

I then cut some small holes (about .4" diameter). and the torch wants to dive hard into the plate. I turned off THC and set cut height to .0625, the voltage that it reads is 151 or above. The hole looks good, but i'm just wondering why the voltage would be higher?

I then go back and do a straight cut, and its back to 141

I have the ground directly on the stock.

Any thoughts? I'm thinking about just cutting these holes without THC. is there a way to turn it off mid program?

[Mike 1948]

If the actual voltage is higher than the operator set voltage, then a signal is sent to the z axis drive to raise the torch until the two voltages are the same. Consequently if the actual voltage reading is higher than the set voltage, the z axis moves the torch closer to the plate to make both voltages equal.

The arc voltage is a stable method of monitoring torch height, but only at a fixed cut speed. When the machine slows down, the plasma arc continues cutting at a fixed power level, this causes the arc voltage at the torch to increase as it is burning a bit of a wider kerf....so when the voltage increases on a speed slowdown, the THC adjusts the actual voltage by moving the torch closer to the plate. When the slowdown is substantial, the torch can actually hit the plate. There needs to be a height freeze in these situations, and I'm sure there is a setting in your system, and I'm sure Torchead can help with it, that has the ability to eliminate diving in corners and on small features.


Jim Colt Hypertherm

Hi Guys,
Just when I thought I had a handle on this I am confused again.
"If the actual voltage is higher than the operator set voltage, then a signal is sent to the z axis drive to raise the torch until the two voltages are the same. Consequently if the actual voltage reading is higher than the set voltage, the z axis moves the torch closer to the plate to make both voltages equal." Seems contradictory???? I'm hoping its a typo.
I'm still trying to wrap my head around THC. I've had(have) problems on long sweeping arcs where the torch raises up away from the material to the point it does'nt cut through. I wonder if my up and down pins are reversed. I have a couple of questions to get my head on straight.

1. If I raise my set volts on a long straight cut with THC will it raise or lower my cut height?

2. If the actual cutting voltage is higher than the set voltage, the torch will move down to get to the set voltage: Yes/No

3. If I slow down, the cut voltage goes up; if I speed up cut voltage goes down: Yes/No

The more I type the more confused I get.
Help:drowning: and Thanks

Mike

[jimcolt]

Mike,

Sorry for confusing you....you must have read my post before I went back and read it over....you will notice I corrected it shortly after posting! It should have read (and does now) "If the actual voltage is lower than the operator set voltage, then a signal is sent to the z axis drive to raise the torch until the two voltages are the same. Momentary dislexya.

Your questions: 1. If you raise the set voltage while the torch is cutting straight...the tHC will raise the torch. Higher voltage = higher torch. Rule of thumb.....1 volt of change in setting is approx .005" of physical height change.

2. If actual cutting voltage is higher than set voltage....the torch will move down. Lower voltage = lower torch.

3. If you monitor the arc voltage while the torch is cutting along at a fixed height.....then you slow the cut speed down....you will see the voltage increase. If the height control is active...the torch will get closer to the plate as it is compensating for the higher voltage. The opposite will happen with a speed increase.

It can be a little confusing...I started working with arc voltage height controls in 1978......and I still posted the concept in reverse!

Just try to remember that a longer arc results in a higher voltage. The torch height control is measuring the voltage right acroos the output of the plasma power supply....from the electrode to the plate. The plasma power supply has not control over voltage, rather it controls current (amperage)....so the voltage is completely dependant of the length of the plasma arc....but under constant conditions (cut speed, air pressure, nozzle and electrode wear, etc).

If you have your polarity reversed (I have done this more than once)....the torch will do one of two things: It will either rise until the arc goes out, or it will lower until it hits the plate.

Hope this helps a bit.

Jim

Hi Guys,
Just when I thought I had a handle on this I am confused again.
"If the actual voltage is higher than the operator set voltage, then a signal is sent to the z axis drive to raise the torch until the two voltages are the same. Consequently if the actual voltage reading is higher than the set voltage, the z axis moves the torch closer to the plate to make both voltages equal." Seems contradictory???? I'm hoping its a typo.
I'm still trying to wrap my head around THC. I've had(have) problems on long sweeping arcs where the torch raises up away from the material to the point it does'nt cut through. I wonder if my up and down pins are reversed. I have a couple of questions to get my head on straight.

1. If I raise my set volts on a long straight cut with THC will it raise or lower my cut height?

2. If the actual cutting voltage is higher than the set voltage, the torch will move down to get to the set voltage: Yes/No

3. If I slow down, the cut voltage goes up; if I speed up cut voltage goes down: Yes/No

The more I type the more confused I get.
Help:drowning: and Thanks

Mike

[Mike 1948]

Thanks Jim,
I think I understand it now.
Slower speed or longer arc= higher cut voltage.
Wow, it only took me 2 years to get that through my pea brain

Thanks Again
Mike

[Torchhead]

been reading and re-reading alot of these posts, plus being doing a bunch of practice. Things are starting to come together! thanks everyone for the help.

i do have one new question though

tonight i was doing some 3/8" steel. 60amp tip. about 41ipm.

when doing a straight cut, the voltage is a perfect 141. I verified this by turning off THC, setting cut height and making a straight cut.

I then cut some profiles using the THC, and again things were great.

I then cut some small holes (about .4" diameter). and the torch wants to dive hard into the plate. I turned off THC and set cut height to .0625, the voltage that it reads is 151 or above. The hole looks good, but i'm just wondering why the voltage would be higher?

I then go back and do a straight cut, and its back to 141

I have the ground directly on the stock.

Any thoughts? I'm thinking about just cutting these holes without THC. is there a way to turn it off mid program?

There are a couple of things that can help you in the DTHC settings and MACH.

The "TIP SAVER" is a voltage based anti-dive that will lock the Torch down moves if the voltage starts climbing above the preset % in the Cut Profile settings. Example: You have the Preset value (target) at 141 and the TIP SAVER at the default 2%. That would cause the DTHC to stop DOWN moves if the voltage reaches about 144 VDC. It's really meant to prevent torch dives at the end of a cut but will lock anytime the voltage moves up above the percentage. It's annoying if you are making a cut that really needs to have higher voltage (like a small hole cut or really slow movements). It can be turned off or the value raised to 10% basically disabling it.

The other setting is in MACH and is motion based anti-dive. The Anti-Dive setting allows you to enter a percentage based on the feedrate. What that means is you can select a number that if the feedrate drops below that percentage, MACH ignores the inputs from the DTHC (locks the Z). Properly selected it can be used to stop head dives on small holes and acute angle cuts where the machine naturally slows down. The slippery part is that the acceleration of a given table defines how fast it can move in a tight turn. The slower, heavier the machine (gantry), the more it will slow down. You just have to put in numbers that will work for the type of cut it is. You can turn the Anti-dive in MACH on/off with the button.

Finally there is a way to turn the THC function ON/OFF in MACH from G-Code. I have attached two MACH Macro's that will, if placed at the right spot in the G-code disable the THC logic (same as turning off the THC Button in MACH) and/or turn it ON.

To test put them in the Macros Folder under MACH in the Folder name that matches the profile you are running. Use the MDI screen and type in the M101 and M102 codes and do back and look at the THC Button LED on Program Run. You should be able to control the button with just the two codes.

Process the smaller holes as a different layer in SheetCAM and drop the feedrate to less than 1/2 the normal for that material and turn off the THC (then back on at the beginning of regular cuts). Do it manually in g-code by using a Code Snip when you build the processes, to see if it helps then contact me and I will modify a post so you can easily pick a plasma tool number and it will automatically turn off the THC button (and back on at the end)

By making the smaller holes a different layer and a different cut process you can change how the machine cuts the smaller details.

Plasma cutting is not a precision machining process and cutting holes with a diameter of less than 2X the material thickness is more like shooting it with a bullet than slicing with a scapula

TOM caudle
www.CandCNC.com

[jimcolt]

Good advice as usual from Tom....one of these days I need to get familiar with the mach software so I can help answer these questions.

One other thing....not all plasma systems have issues with cutting holes under 2x the plate thickness. The latest technology with high definition plasma from Hypertherm produces 1:1 holes from 1/4" thick steel to 1" thick steel with no taper, and no ding and divot (lead in , lead out anomalies)....the new process is called TrueHole.....and it uses a very aggressive oxygen plasma and oxygen shielded arc only for cutting holes. Unfortunately it is only on the high end (read expensive) systems today....maybe someday in the future we will be able to bring the technology over into the air plasma systems!

Jim

[Torchhead]

Good advice as usual from Tom....one of these days I need to get familiar with the mach software so I can help answer these questions.

Let me know when you want to start building your own plasma table and I'll furnish you the interface and DTHC electronics! Come on over to the Dark Side:stickpoke

Tom caudle
www.CandCNC.com

[jimcolt]

Tom,

While I personally will likely build another table or two in my lifetime (I have built two to date!), Hypertherm will not. Hypertherm sells our products to everyone that builds cnc tables....competing with them (by building machines) would probably not be the best business decision!

I actually have been thinking about building a table in my home shop, using your products....to familiarize myself with Mach, stepper drives, and your THC technology...primarily so I can help more of the users on these sites.

Jim

[Torchhead]

The offer is to Jim Colt (individual) for your own table and for , as you state: familiarize yourself with our products and the MACH3/SheetCAM combo for plasma cutting. Like Hypertherm we don't build tables or mechanical parts for CNC. A lot of my business is to OEM's that build and sell tables and I have no intention of competing with my customers!

Contact me any time.

TOM caudle
www.CandCNC.com

[multiplex]

thanks again for all the info guys.

one thing i'm struggling with is deciding what the capability of the machine are. Specifically related to cut draft and lead in / lead out divots.

i've tried a number of different combination of lead in (on interior cuts), and various lead outs but still seem to have poor quality at the start point. But then again what should i consider poor to be?

I also seem to get more draft than expected even on thinner stock (1/8", etc). Maybe i'll have to measure the angle and report back.

Does anyone have photos of what could be expected as the best hole, slot , profile that can be cut using an air plasma torch in various materials?

[jimcolt]

If you want to email me I can send you a slide presentation of best practices for hole cutting. It will be a .pdf file with a few slides suggesting lead ins, overburns, what to do with height, etc. The presentation is aimed at high end oxygen plasma systems, but it works equally well with air plasma....assuming you have a good operating torch height control as well as a machine that has minimal backlash and relatively good accelleration.

Jim [email protected]

[multiplex]

recently i've been doing a bunch of cutting with the fine tip, which has been working well.

I've noticed i sometimes get a serrated cut (almost like a fine kitchen knife).

is this from moving too slow? too fast? or maybe i need to change my consumables?

[multiplex]

ok a little update to my question.. i investigated my machine and found a few mechanical things that might have been contributing to vibration in the machine.

for one, the pinon gear on my gantry was rubbing the structure (leaving imprints from the teeth)

the big factor though effecting the cut is the DTHC. it seems to have a very fast / erratic motion when trying to maintain torch height. the quick motion causes the torch to vibrate.

I need to add some bracing on my Z axis (k2 assembly), but i'm wondering what controls the speed that it corrects at?

would this simply be in my acceleration / motor tuning? or is there another setting specific to the torch control?