Mach3 Step By Step

[brouser1]

Hello,

Let me start out by saying I am a beginner and need some help. I have built a cnc plasma table. And I am very close to actually cutting.

I have loaded my g code. My machine is sitting at 0,0,0. Before I hit RUN, how does my machine know where to start cutting? I need to tell the table the table the X & Y coordinates of my material to be cut, right? I know this is probably a stupid question, but I can't find any tutorial that have shown this step.

Thanks,

Eric

[H.O]

Hi,
Jog the machine to the corner (or center or whatever) of the material that coresponds to part zero in your program. Now zero the X and Y axis with the zero buttons on the screen. Load your part file or click Regen right under the graphical toolpath window if you already have it loaded.

/Henrik.

[Torchhead]

Positioning of cuts versus table 0 are best done in the CAM program. If you always start from a known Home position then if something happens you can rewind and get back to where you were exactly. When you use the move to a point and zero (arbitrary work zero) you can lose position and have a devil of a time finding that work zero again to start from. If you always work from a table zero that you are get back to with accuracy, then you can always cut relative to that. CAM programs like LazyCAM and SheetCAM let you define a table zero, a material position relative to table zero and then place a "part" anywhere on the material and everything is measured in absolute from Table zero. You can return to table zero and recalibrate the position using the Reference and XY home switches.

For a milling machine that might have movable fixtures and where work is usually referenced to the edges of the the blank, then setting it as a work zero makes sense. You perform a precision touch-off to establish the work zero (not just your eyeball) so getting back accurately is possible.

First time you are cutting along and have to hit e-stop or the power takes a glitch and you lose position, and then try to reestablish a cut from some spot you eyeballed as zero you will see what I am talking about (:-0

TOM caudle
www.CandCNC.com

[H.O]

Hmm...I may be missing some plasma specific thing but when pressing the zero-buttons in Mach3 you are effectively setting the current part/fixture offset (G54, G55 etc) from from the table/machine zero to the part/fixture zero.

In case you do loose position all you need to do is reference the machine, select the correct offset (G54, G55 etc) and then G0 X0 Y0 and you're back to the "arbitrary" zeropoint - no matter if you originally eyeballed it or found it with a Renishaw probe.

If the power goes down before you've been able to save the offsets then you might have a problem but honestly, how often does that happen.

Anyway, which ever way works for the application and user is the best.

/Henrik.

[brouser1]

Great, I think I understand how this works a little better. I think I will go with the constant 0,0

My next question with Mach is:

With my floating Z axis, I would like to have the Z home 3" above the material (just seems like a safe height). I can jog the Z up to the 3" position then hit Zero (isn't this zeroing the Z axis? If not, do I zero the Z axis on my machine?) Right now if I hit the REF Z button it will slowly goes down, touches the table, but then it doesn't raise up 3"

Where do I set this? The set the X & Y with a -.5 and it does what is suppose to do, goes to the switch then reverses back out .5" Something doesn't seem to work the same with the Z axis.



Thanks
Eric

[H.O]

Hi,
No, I don't think it's actually doing what you think it does... When you set a home-offset distance in Mach3 it is the value that the machine coordinates will get set to when the homing is done - the machine will not automatically move away that amount.

Homing works like this: Find the switch - reverse until switch is cleared - set/reset the machine coordinate for the current axis. If no home-offset is set the spot where it clears the switch will be machine zero. If the home-offset is set to 0.5 the machine coordinate will get set to 0.5 at the spot where the switch clears meaning you are 0.5 away from machine 0.

Zeroing an axis is not the same as homing an axis. When homing you are finding the machines zero or reference point off of which all offsets (part zeros) are based. When zeroing (ie. pressing the zero button or entering a value directly into the axis DRO) you are establishing an offset between the "machine zero" and the "part zero". In other words you are setting part zero. Having a repatable machine zero is what will let you go back to previosuly defined part zeros - if the machine zero moves, so does ALL you part zeros/offsets. (G54, G55, G56 and so on) - not good, usually.

If you go to the diagnostics page in Mach3 you can see the DRO's for machine coordinates, offset and part coordinates, if you jog around a bit, zeroing here and there you'll see how the numbers adds up.

Now, I don't know how this floating Z-axis works and if it's part of a THC system etc, hopefully Tom will jump in there. But if "home" for the Z-axis is where the tip touches the table/material and you really want to have your machine zero 3" above that point. Then enter -3 in the home offset. If you want it to automatically move up those 3 inches you'll have to edit the homing script, it's no big deal but lets not go into it before you know that is what you really want.

Having a floating home/machine zero like this seems awkward to me - but then again, I'm not used to how a plasma machine normally works so I may be way off - in which case I apologize.

/Henrik.

[Torchhead]

Now, I don't know how this floating Z-axis works and if it's part of a THC system etc, hopefully Tom will jump in there. But if "home" for the Z-axis is where the tip touches the table/material and you really want to have your machine zero 3" above that point. Then enter -3 in the home offset. If you want it to automatically move up those 3 inches you'll have to edit the homing script, it's no big deal but lets not go into it before you know that is what you really want. Having a floating home/machine zero like this seems awkward to me - but then again, I'm not used to how a plasma machine normally works so I may be way off - in which case I apologize.

Plasma cutting, unlike most other cutting processes, is done on material that moves from warping and heat stresses. Since the top of the material is considered Z zero, it's not like a process where you can set it once and forget it. You need a method called Initial Height Sensing (IHS). It "feels" for the top of the material and reestablishes Z zero. Plasma is done floating above the material. Piercing (like blowing a hole in a brick wall with an RPG round) is done as high as possible to prevent molten blow back of metal from clogging the tip. Cutting is done at a fixed gap (often 1.5mm or less) above the material at speeds that are too quick for a human to control on warped material.

The presence of a Home on Z where it's not in relation to any measurement of Z zero is less than useful. You can't work with a zero 3" up in the air. Too much math for when you need to pierce at 3mm above the material, plunge to 1.5MM, let the Torch Height control it UP and DOWN, and then going to the next pierce point where the material height could be 12mm different than the starting point. You don't give the plasma torch depth commands in the CAM program. It instead has "height" commands that are automatic and measured above the top of the material (Z zero). Applying an offset from some moving point 3" above the changing material would take some fancy code.

The simplest way to raise it up to 3" is to just tell it to do that at the end of the cut. It may not be exactly 3" but the new Z zero gets reset on the next "touch-off". In a CAM program you can assign a rapid height parameter and it puts the lift at the end of the cut automatically.

The distances in plasma are critical. If you need to pierce at 3.0 mm and start the cut at 1.5mm then you need to be within 5% of those numbers for good cuts.

The use of the floating torch holder to be the "probe" and the Z homing move to set the zero (and apply the switch offset) is a reliable and low cost method. There are other ways but they all end up doing the same thing: Find the top of material and reference the Z to get accurate pierce and starting cut height.

It's not impossible to work with offsets in plasma cutting but you won't find plasma programs that will work in negative Z numbers and plasma is hard enough as it is. A lot of people don't believe it, but doing plasma cutting RIGHT is harder than most other cutting processes.

TOM caudle
www.CandCNC.com

[H.O]

Thanks Tom,
It's pretty much what I thought and I think you and I are on the same page here. Machine zero (home) for the Z-axis is a fixed and repeatable point on the Z-axis slide. Part zero is the top of the material (this, per definition, does indeed set a part or fixture offset) and you can reset part zero at the start of each cut if the material warps etc.

You won't see negative Z-coordinates as long as you don't drive the tip thru the surface of the material.

The use of the floating torch holder to be the "probe" and the Z homing move to set the zero (and apply the switch offset) is a reliable and low cost method.

I guess the thing that is not yet really clear to me is if you're using the floating head to set part zero or machine zero (home). If part zero then it's completely logical and exactly as I thought, if you are setting machine zero (home) at to the top of the material then it's not as I thought and still seems very awkward to me but I know you know the plasma stuff so I'll leave it at that.

/Henrik.

[Torchhead]

A 'table zero' up the slide on Z serves no purpose what so ever. You can only have one home per Axis. Since the Z ref in the touch off is a homing move it establishes home as the top of the material not some arbitrary point up in the air. On a plasma table you do not typically do a 'home all' (go home). We in fact have a custom screen button that is a REF XY and moves the Z up 1" above the current Z zero.

Homes are to establish a known position on the machine (repeatable) to reference to so you can run absolute cuts or offset cuts. Having a home up the air a varaible distance from the top of the work serves no refeerence function other than to be able to raise the Z up to the same point on the slide. If you then use that as a Table zero you have to go through an extra step and re-establish the top of material as the work zero. To me that is awkward to me. Having a single step method to do that automatically in the CAM (G-code) without writing macros and using a probe input and wasting an input seems to be a more straight forward way to do things.

You have to realize that plasma cutting is not a precision process and happens very fast and dramatically. The operator does not need the same skill level as a VMC driver and things like having two coordinate systems, fixtures, offsets, and multi-pass cutting are foreign concepts. That being said the added moves in plasma (IHS, Pierce delay, plunge to beginning cut height, lead-ins and things like anti-dive on corners and ends) makes the plasma process more complex overall if they are not handled automatically.

TOM caudle
www.CandCNC.com

[brouser1]

Thanks again for all the info. My original request of 3" was just my perceived "safe" height. Anyway, Tom if you can help me with what you said:
We in fact have a custom screen button that is a REF XY and moves the Z up 1" above the current Z
Right now I hit the REF Z button and it touches the surface and stops. Please tell me what to change back or what to check to get the 1" above the current Z. Since mine is not working, I am sure I must have checked, unchecked, or somehow messed something up?

Thanks again.
Eric

[Torchhead]

When you hit a manual REF in MACH it does just that: moves to the Home switch, stops backs up to clear the switch and stops.

What are you trying to do? REF is used to find a known position on the table. On Z that is top of material. If you want it 1" (or 3" ) above the table you have to tell it to do that in G-code.

On startup, the best procedure is to load some material, do a manual REF one time on XY and Z and then raise the Z with a jog. From that point forward the g-code from your CAM should control the rapid heights, pierce heights and beginning cut height. If you want the rapid height to be 3" then put that parameter in your CAM (SheetCAM?) as a Table Parameter.

The Z will not automatically raise to Safe Z with a REF move. It would not help much even if it could because Z REF is an integral part of the touch-off move and would waste a LOT of time on every touch-off raising back to Safe Z (Rapid Height) THEN plunging back to Pierce height. That gets old in a hurry.

Let the G-Code control your machine. If your POST is setup right all of that stuff is totally automatic including the touch-off (REF Z) and with SheetCAM even the FREQUENCY of the touch-offs based on XY distance.

TOm caudle
www.candcnc.com