How do you pick "home"?

[lilricky2]

I am not sure how to phrase this question, so I hope spmeone understands enough to advise me. After I make my part drawing, I import it into Mach2. When I start up, the spindle picks up and goes to a "home" location. It then plunges at whatever speed I set the z-axis to whatever depth I chose to make the first pass and starts the cut. I guess my question is this. why the hell does it do this? It's getting old chasing the endmill around with dial indicators and trying to extrapolate a starting point. It would be nice to put my piece in the vise set the mill at 0-0-0 and have it plunge and start the pass. I was in the petrochem industry as a manual machinist for 22 years, but I am a complete cnc idiot. Soren's videos helped, but the Bobcad training videos were a complete waste of time and money. I have Bobcad versions 19, 20, and 21 and am ready to give up on the whole damn idea. I am running an older version of Mach2 as I am afraid to upgrade for fear of really being confused. Someone, please help me before I take a plasma cutter to a $5000 cnc conversion.

Thanks for any help,
Rick

[Kiwi]

Please supply a screen shot of your part in BobCad and the first few blocks of your code.

[judleroy]

Bobcad has a tendency to write G00 X0 Y0 and Z at whatever your rapid height is at the beggining of a program. You may have to edit your G-code.I've never used mach2 but are you zeroing out your X and Y where you set your tool. I'm guessing where you set your tool you want too be 0,0.

[tobyaxis]

Originally Posted by lilricky2 I am not sure how to phrase this question, so I hope spmeone understands enough to advise me. After I make my part drawing, I import it into Mach2. When I start up, the spindle picks up and goes to a "home" location. It then plunges at whatever speed I set the z-axis to whatever depth I chose to make the first pass and starts the cut. I guess my question is this. why the hell does it do this? It's getting old chasing the endmill around with dial indicators and trying to extrapolate a starting point. It would be nice to put my piece in the vise set the mill at 0-0-0 and have it plunge and start the pass. I was in the petrochem industry as a manual machinist for 22 years, but I am a complete cnc idiot. Soren's videos helped, but the Bobcad training videos were a complete waste of time and money. I have Bobcad versions 19, 20, and 21 and am ready to give up on the whole damn idea. I am running an older version of Mach2 as I am afraid to upgrade for fear of really being confused. Someone, please help me before I take a plasma cutter to a $5000 cnc conversion. Thanks for any help, Rick

You have to set a Work Position Coordinate in your Mach 2 with and Edge Finder. G54-G59. This is done by inputing the machine position numbers like this.

Assume your machine is in the Machine Home Position X0 Y0 Z0.
Jog the X Axis to your Part Program Origin
Lets say that number was X-15.0000
Now do the same with the Y Axis
Lets say that Number is Y-8.5000

The Z is set by the Top of the work Piece
Lets say that is Z-4.5000

On a Work Position Offset Page for your G54 it would read like this.

G54
X-15.0000
Y-8.5000
Z-4.5000

Your part Home position should be a Corner X0Y0 or Center X0Y0


If you still don't understand sent me a PM and I'll call you later

Cheers!!!!

[ger21]

Originally Posted by tobyaxis You have to set a Work Position Coordinate in your Mach 2 with and Edge Finder.

You can also jog over to where you want 0,0 to be and zero the axis. IF the actual 0,0 position isn't that critical.

[HuFlungDung]

How do you pick home? If you are programming in absolute coordinates (which you should), then fundamentally, you must have the part located on the CAD axis so that the X0Y0Z0 point on the part corresponds to X0Y0Z0 on your machine. You set your controller into absolute mode by writing a
G90
into your program, near the beginning, before any axis movements are commanded.

This correspondance of position is the primary step to visualize.

Machine zero is by nature defined as G53 X0Y0Z0. G53 is the machine coordinate system, and cannot be altered. Everything else that we do with work shifts and tool offsets is simply a temporary adjustment that is piggybacked on top of the machine's coordinate system. The controller keeps track of these shifts for us, so that we can if we choose, have a make-believe (virtual) coordinate system X0,Y0,Z0 wherever we wish.

Then, as Tobyaxis described, it is usually necessary to install and call a workshift in your program, because chances are, that wherever you plopped the part down on the table, the reference point on your part (as visualized in CAD), does not actually correspond with machine zero, which your machine establishes after homing during the power up stage of getting the machine ready to work.

You can call which workshift you want to use in your program. The work shift most commonly used would be G54, but there are additional ones available, if needed. However, installing values in the workshift register (a table of positions stored in your controller) is not usually done within the context of your actual program. As Toby said, you use manual jogging procedures to move the spindle to the zero point of your part. When it is exactly over X0Y0, then you are ready to note the display coordinates, as they should at that moment, be showing how far your have jogged from the machine zero. Those values are then entered manually into the G54 work offset register.

So near the beginning of your program, then you would command
G54
in order to instruct the controller to pretend that the coordinates you entered in the G54 register will become the temporary X0Y0 for the commanded absolute movements that follow.

Setting tool length offsets adds an additional complexity factor to this whole scenario. For the sake of clarity, I advise users to set all their tools to a reference block that is at least as high as the top of the part. Why? Well, the clearest methods of programming always assume that Z0 is the top of the part. This makes it much easier to visualize what is happening to the current tool, ie., absolute commands that are Z- will put the tool into the work zone, versus Z+ commands will imply that the tool should be in clearance above the part.

If you use a tool setup block that is higher than the top of the stock, then you can touch all tools off the top of this block. These values are entered in your tool offset register, one for each tool, and the purpose of this is to make all the tools seem to have the same length when called into use in your program.

So, if the tools are now all set, there will still remain a small discrepancy to account for, and this would be the difference between the height of your tool setoff block and the actual top of your work stock.

On a Haas, I measure this distance using any one of my tools, probably immediately after the last tool length offset I measured. The last tool is touching the setoff block, so now I go to a screen on the display that allows me to temporarily zero the Z axis on the display. Then, jogging from the setup block height, to the top of the work stock should result in some number and this value is a measurement of the amount to be entered into Z column of the G54 work offset. So that accounts for the last offset to be made.

For a beginner, or even an advanced user, it can be good practice to command
T1 M6
G43 H1 <--length offset call for Tool 1
G00 G54 X0 Y0 Z1.
as the first movement in your program immediately after your tool call.
What this will do is move the table to park the tool over the reference point that is recorded in the G54 offset table. If you can turn down the Rapid speed before executing that line, then you will observe the tool moving to the reference point, with the tip of the tool 1" above the top of the stock. This will give you visual confirmation that the settings are correct. Practise this with one hand over the RESET or ESTOP until you are confident in what is going to take place

[InspirationTool]

What HFD said....

I have been picking the back right corner of my part as 0,0,0. That means the part is completely in the negative coordinates. But as it's easy to put a work stop on the back right of my vise, it works out well. It also means I can machine different size parts without changing my origin.

-Jeff

[lilricky2]

I tried to import some screenshots. I've done it before but I just can't remember how I did it. Let me work on it and I'll see if I can post them later.

Rick

[Kiwi]

To capture your screen use "Print Screen" key then paste into "Paint" or whatever.

I don't know Mach2, but looks like you need to enter your part origin XYZ into G54 table.

[tobyaxis]

Originally Posted by lilricky2 I tried to import some screenshots. I've done it before but I just can't remember how I did it. Let me work on it and I'll see if I can post them later. Rick

Control + Alt + Print Screen if you want a smaller window.

Cheers!!!

[The One]

Rick,

When you are stting up your program in BobCAD you will have to do a few things:
1) Make sure that the part is oriented over the area you want to machine within. If you want the center of the part at X, Y 0 then do so. If you want the bottom left hand corner over X, Y 0 then set it up that way in the CAD window.
2) Make sure that your UCS is not rotated or shifted anywhere in the CAD Screen.

After that you will generate your program and load it into Mach2.
Jog the machine to the location you want to be 0,0,0.
Then press the Zero X, Zero Y and Zero Z buttons in the Mach2 interface. This should setup your Work Coordinate system.
Then start the execution of the program.

To be on the Safe Side: If you apply this method you will want to make sure you remove any G53-59, G49 and G43 commands from the program. They tend to change the Offset Values or the Coordinate system.

Regards