plunge rate ? in sheetcam

[HammerDownJustin]

I am new to this and working with my table..Im still getting some dragging from my thc..but main question is what is a good rule of thumb on the plunge rate? I am running candcnc electronics with a hypertherm 65 and shielded 65amp tip right now on 3/16" plate while testing..im getting a dryer this week and noticed some moister in my air hose so it might be messing with the thc and the metal was 20 year old red iron plate slightly rusty

[I Lean]

I don't know if there is a rule of thumb, but I have mine set at 100 IPM also. It only controls how fast your torch will move from your rapid height, down toward your pierce height. (or toward your initial height sensing)

[BTA Plasma]

Also don't forget to go to config/homing limits in Mach3 and change your Z axis home speed from 20% to 100% to get the full 100ipm.

[HammerDownJustin]

Dangit I forgot to change the 20%...thank everyone for there help

[beefy]

I just set mine the same as the feedrate or even faster if the feedrate is a slow one. Your pierce delay gives time for the torch to blow a hole through so if the plunge rate was slow then effectively it's like the pierce delay being extended. This could potentially cause a loss of arc if the pierce hole gets too big.

My thinking is once the hole is made, get the torch down to cut height straight away so the hole doesn't get too big.

A few weeks ago I actually had to slightly reduce the pierce delay when I got a lost arc condition at the pierce hole. I noticed the pierce hole was quite large and I'm guessing this is what caused the lost arc. Reducing the pierce delay gave me a smaller hole which would have allowed the arc to keep contact. Never got a lost arc after that.

Keith.

[beefy]

Also don't forget to go to config/homing limits in Mach3 and change your Z axis home speed from 20% to 100% to get the full 100ipm.

I'm also running Candcnc electronics / Mach and this is news to me. What has the homing speed got to do with plunge feedrate. Isn't the homing % only for the speed at which the axis travel when doing a homing operation. It shouldn't affect normal feedrate commands, and the plunge move is not a homing operation.

Keith.

[abmagrum]

I set mine at 150.

Go to archlight plasma table click on training watch the videos its free.

Scott explains how to set everything up .

I am new to this and the videos show you how to set everything up. feed rate, amps, thc height ,etc

hope this helps

Al

[HammerDownJustin]

Will check the videos out thank you...what made me wonder is sometimes my thc doesn't raise quick enough and my torch will drag..thc volts look good when cutting..using hypertherms recommend settings

[BTA Plasma]

Also don't forget to go to config/homing limits in Mach3 and change your Z axis home speed from 20% to 100% to get the full 100ipm.

I'm also running Candcnc electronics / Mach and this is news to me. What has the homing speed got to do with plunge feedrate. Isn't the homing % only for the speed at which the axis travel when doing a homing operation. It shouldn't affect normal feedrate commands, and the plunge move is not a homing operation.

Keith.

Welcome to the fine details Keith. When your touching off or travelling in Z to find home your using the percentage set in Mach 3. Set it to 100% and you will be amazed. So travelling down to the top of the plate is setting Z home with Mach.

[BTA Plasma]

I set mine at 150.

Go to archlight plasma table click on training watch the videos its free.

Scott explains how to set everything up .

I am new to this and the videos show you how to set everything up. feed rate, amps, thc height ,etc

hope this helps

Al

That must be with the 380oz motors. That is still pushing it to the edge of loosing steps with a 5tpi screw.

[beefy]

Correct me if I'm wrong but the plunge rate setting in Sheetcam does not control how fast the torch moves from the rapid height (or safe Z).

In Sheetcam the plunge rate is how fast the torch moves from the pierce height to the cut height, which in the example below is from 4.5mm to 1.5mm. Look at the following gcode portion from my latest file generated by Sheetcam:

G00 Z70.0000 Rapid to safe Z height of 70mm
G00 X156.4147 Y346.4676 Rapid to next pierce location while torch at safe Z
G28.1 Z15.00 F500.0 Touch off - Z rapids down to 15mm then moves at a feedrate of 500 m/min to touch
off on the Z home switch (these settings are entered in the post processor)
G92 Z0.0 Zero Z dro
G00 Z0.8800 Rapid to 0.88 mm (switch offset - set in post processor)
G92 Z0.0 Zero dro - touch off complete, torch at top of plate
G00 Z4.5000 Rapid to pierce height
M03 Torch on for pierce
G04 P1.2 Pierce delay time for torch to burn through.
G01 Z1.5000 F2000.0 THIS IS THE PLUNGE RATE HERE where Z goes from pierce height to cut height.
2000 mm/min is in my plunge rate box.

I think the Mach homing operation is being confused with Sheetcams plunge rate setting which are completely separate and different things. The homing % setting is to stop the homing being done at a high speed. The axis should not fly into the home switches at warp speed.

What % setting you have in Machs config/homing limits has no bearing on Sheetcams plunge rate. It simply sets how fast an axis looks for the home switch. A touch off operation with gcode produced by Sheetcam works differently to a basic axis homing opertion, as the code above shows.

Keith.

[BTA Plasma]

Correct me if I'm wrong but the plunge rate setting in Sheetcam does not control how fast the torch moves from the rapid height (or safe Z).

In Sheetcam the plunge rate is how fast the torch moves from the pierce height to the cut height, which in the example below is from 4.5mm to 1.5mm. Look at the following gcode portion from my latest file generated by Sheetcam:

G00 Z70.0000 Rapid to safe Z height of 70mm
G00 X156.4147 Y346.4676 Rapid to next pierce location while torch at safe Z
G28.1 Z15.00 F500.0 Touch off - Z rapids down to 15mm then moves at a feedrate of 500 m/min to touch
off on the Z home switch (these settings are entered in the post processor however mach takes over % of speed because of the G28.1)
G92 Z0.0 Zero Z dro
G00 Z0.8800 Rapid to 0.88 mm (switch offset - set in post processor)
G92 Z0.0 Zero dro - touch off complete, torch at top of plate
G00 Z4.5000 Rapid to pierce height
M03 Torch on for pierce
G04 P1.2 Pierce delay time for torch to burn through.
G01 Z1.5000 F2000.0 THIS IS THE PLUNGE RATE HERE where Z goes from pierce height to cut height.
2000 mm/min is in my plunge rate box.

I think the Mach homing operation is being confused with Sheetcams plunge rate setting which are completely separate and different things. The homing % setting is to stop the homing being done at a high speed. The axis should not fly into the home switches at warp speed.

What % setting you have in Machs config/homing limits has no bearing on Sheetcams plunge rate. It simply sets how fast an axis looks for the home switch. A touch off operation with gcode produced by Sheetcam works differently to a basic axis homing opertion, as the code above shows.

Keith.

[beefy]

Hi BTA,

I'm getting some more info on this one because there are some things I'm not 100% certain on.

I'm noticing in forum searches, not many users are putting a ref speed in their Sheetcam post processor as I have so if they have G28.1 Z15 then the torch would rapid down to 15mm then home (touch off) at a speed determined by the % setting in Machs Config / Homing Limits box.

My guess is that when F500 is put on the end of this gcode line it overides Machs homing speed, otherwise why would Sheetcam give this option if it didn't work.

Back to the % setting in Config / Homing Limits. Isn't it dangerous to set this to 100% because won't any homing operation be done at the machines rapid speed, possibly smashing the homing switches or whatever. A homing operation is to find the switch which Mach doesn't know the position of so there's no deceleration as it get near the switch, it just goes at the homing speed until if finds it. And in a touch off operation such as G28.1 Z15 the Z axis will rapid down in any case to 15mm then slow down to the % homing speed, so there's not a great distance to cover in any case.

Keith.

[BTA Plasma]

Yes that is correct Z homing rate is what Mach 3 config/homing limits gives a percentage of. The F500 is redundant in that it only works in that line if there is a G1, G2 or G3. However a F number is stored in Mach so that the next G1 will be at that preset F number if no other F number came after it. If your seeing an F number from sheetcam you must have a version that changed the post or you using a post that uses that feedrate without a G1. We use as a default 80% speed. If your Kernal speed is 45K or greater you can use in excess of 150ipm feedrate for Z touch off. The reason it works is that the screw is a mechanical advantage to slowing the Z axis down. Without the mechanical advantage lost steps would occur and your pierce height wouldn't be ideal.

[BTA Plasma]

Sorry I don't mean to confuse you. We tell a customer that at the beginning of their plasma cut day get your toch about 1" off the material and set z zero. This way their isn't a value set in there from them or an employee messing with Mach. This means the initial Z home move is at 80% from 1" up. Does that make more sense?

[beefy]

Hi BTA,

I've asked on the Sheetcam forum about the feedrate at the end of the G28.1 line. However Sheetcam put it there, it's still just a gcode command to Mach so now I'm at the point of learning if this overides the default homing speed set by the % value in Config / Homing Limits. Now that you've told me about this F500 only working if there's a G1/2/3 in the line, I have something else to research (when does it end ). Seriously though I love it when I learn a bit more "inside information" as I like to call it. If it doesn't overide Machs % setting I'll do away with it and just set the Z homing speed in Mach.

I think I get what you are saying about the fast touch off speed. The 45+ kernel speed allows a higher pulse rate to be sent out thereby allowing faster stepper rotation. The leadscrew on the Z is effectively gearing things down a lot so it's easier for the stepper to stops things very quickly without losing steps, and therefore you can use a faster homing speed. Plus there's not a lot of weight it has to arrest, and the only spinning momentum is the stepper rotor and the leadscrew. I'll probably have a play sometime with faster Z homing speeds and see what the cracking point is where it smashes the microswith or the touch of accuracy starts going bad, then back it off a safety margin. I suppose a fast homing speed over even a 15mm distance could give some time savings on a nested cut with lots of pierces.

I do something similar with zeroing my Z when I first run the table. I just jog the Z down till it's a few mm off the plate and zero it. If I zeroed it 3mm above the plate and the homing distance is 15mm then it will start homing at 18mm the first time.

Cheers,

Keith.

[BTA Plasma]

Outstanding Keith! Your getting a good grasp on some of this. Get to cutting and play with your speed %. You will see where it makes a difference. You are absolutely doing the right thing when you start your initial height a few mm off the plate.

[beefy]

No reply yet on my question on the Sheetcam forum about the F500 in the line of code.

I Googled "mach g28.1" and got a result describing the G28.1 as it applies to Mach. It said the homing operation is done at a percentage of the CURRENT feedrate. That seems to mean the homing speed will not always be the same, it will be slower when the feedrate is slow, or faster when the feedrate is fast.

I was going to trash my method of setting the F500 in Sheetcams post processor, thinking just use the setting in Mach and keep things simple. But if the homing speed does change with different feedrates then the setting in the post ensuers the homing speed will always be consistent.

That is IF the F500 code is not meaningless when there's no G1/2/3 on the line.

So this is why there's whole books written on gcode programming

Keith.

[beefy]

Hi BTA,

got a reply from another forum and so far it's exactly as you said. The F500 on my line of code does not work and Mach still homes at the % setting in Config/Homing Limits.

I'll have to set up some test code and try this out on my table.

I'm glad to have learned something new, thanks for your input.

Keith.