beginner programing help

[Marc Davis]

Ok guys (and gals?)

I have a new (to me) Matsuura MC-560V milling machine with a Yasnac MX2 control. This is my first CNC machine. I'm making good progress teaching myself to program it. I've created a simple program, loaded it to the controller and it runs (in mid air). My problem is understanding all the different origins, offsets, and coordinate systems. It seem to me there may be many ways to skin the cat, but I need a place to start. How are you guys setting things up?

Where is the origin in your Gcode program?
Do you use G52-G59 work cooordinate systems?
If you do, are you programing the offset in to the Gcode with G10 or entering values into the controller manually (and what are you entering)?
How do you set the location of the raw stock relative to the machine and Gcode?
When you set tool offsets, what length exactly are you setting?

Anyone willing to walk me through it?

Thanks
Marc

[dcoupar]

The origin us usually the part datum. I always used G54 - G59 on the Yasnac once the option became available. The Work Coordinate System values are the distance and direction from Machine Zero to Part Zero, i.e. #6516 = -12.1234, #6517 = -7.3343. Some folks used G10 at the start of the program, some entered the values manually.

The Length Offsets can be done in a couple of ways. You can set each tool to the top of the part, or, you can set each tool to a known reference height (like a 123 block) and adjust up or down with the Z of the Work Coordinate system. In either case, the value stored in the H offset is the distance and direction the tool must move from Machine Zero (Z) to the setting point, i.e. H01 = -12.1323.

The Z of the Work Coordinate can be either + or - depending on the direction from the setting point to the top of the part.

Hope this helps.

[Marc Davis]

Thanks for the reply. It does help.

So let me see if I understand.

1) Home the machine
2) Load a program into the machine.
3) Set the tool offsets by touching a 123 block and entering the Z values into the controller.
4) Mount the raw stock into the machine.
5) Use an edge finder to locate the stock in the X,Y.
6) Use a tool with a known offset to locate the Z of the raw stock.
7) set the G54 (work coordinate system) to the X,Y,Z above minus a bit to move the part datum inside the raw stock.
8) push the start button and go make a sandwich :-).

Did I miss anything?

Marc
S

[dcoupar]

Thanks for the reply. It does help.

So let me see if I understand.

1) Home the machine
2) Load a program into the machine.
3) Set the tool offsets by touching a 123 block and entering the Z values into the controller. Your machine may have the TLM Measure and Write buttons for this.
4) Mount the raw stock into the machine.
5) Use an edge finder to locate the stock in the X,Y.
6) Use a tool with a known offset to locate the Z of the raw stock. Or just measure from the top of the part to the 123 block and enter the difference into the Z for G54.
7) set the G54 (work coordinate system) to the X,Y,Z above minus a bit to move the part datum inside the raw stock.
8) push the start button and go make a sandwich :-).

Did I miss anything?

Marc
S

Coffee before step 1.
Single block carefully through the 1st part.

[Jaxbubba]

When I got my first CNC machine, for Fanuc Controls, the set up man told me to Home the machine, go the the RELATIVE position screen and set X,Y,Z all to Zero. That lets you know that when the machine goes to Home Position that the Relative position screen should read X0Y0Z0. You should have green lights on your control that shows you when the machine axis are in home position. XYZ lit, Relative screen reads X0,Y0,Z0 and you are ready to go. Do a tool change to your edgefinder and touch off in X, read the Relative screen
and input that number in the G54 fixture offset table. Input+ -.1 for the edgefinder center and Input+ -.01 to whatever you want to take off the stock for cleanup in X. Do the same for Y and add how much minus you want to take off the stock in Y. For a Fanuc, Yasnac control go to MDI and input the command G28G91Z0; which will take the spindle back to the tool change position. You will notice that the Z reading on the Relative position now reads Z0 again, the X, and Y will still read where you are in relation to the home position. You now have different options for setting your Tools Z height, you can use a 123 block on the top of your stock to set your tools by calling up all the tools you use, and touching off the top of the 123 block with a piece of paper, go to your Height offset table for the tool number used and measure input. Set all your tools that you will use in this program this way.
This makes all your tools 3.00 above your Z0 point on the top of your stock. You then have 2 different ways of telling the control where the true Z0 on the part is. Either input- 3.02 to each tool Height offset number to take .020 off the top of the stock, or take any tool that you have set and touch it off the top of the stock and compare the height offset number to the number on the Relative position screen and take the minus distance difference and put it in the G54 Z offset table then input+ -.02 example how much you want to take off the top of the stock. Since you set all the tools to the 123 block, the control now knows where you want the Z0 to be by setting just 1 tool.Let me know if you need anything else

[Marc Davis]

You guys are both awesome. Thanks for the help. I got some of this working tonight and cut my first part, I'll try out the rest tomorrow.
One other question. For some reason I can't enter the G54 offsets directly. I enter the setting number (#6513) and cursor down to get to the line of the value. I enter a new value and hit write. The value doesn't change. Using G10 to change the values works. My control is an MX3 but my manual is for the MX2. The manual I have talks about a switch in the paper tape reader to protect the settings but mine doesn't seem to have one. I have the protection key switch on the control panel turned off. I'm not sure how familiar you guys are with my exact control but I thought you might have an idea.


Thanks again.
Marc

[dcoupar]

You guys are both awesome. Thanks for the help. I got some of this working tonight and cut my first part, I'll try out the rest tomorrow.
One other question. For some reason I can't enter the G54 offsets directly. I enter the setting number (#6513) and cursor down to get to the line of the value. I enter a new value and hit write. The value doesn't change. Using G10 to change the values works. My control is an MX3 but my manual is for the MX2. The manual I have talks about a switch in the paper tape reader to protect the settings but mine doesn't seem to have one. I have the protection key switch on the control panel turned off. I'm not sure how familiar you guys are with my exact control but I thought you might have an idea.


Thanks again.
Marc

Be careful when changing settings. #6513 is NOT G54 X, it's X minus stored stroke limit. #6516 is G54 X, #6517 is G54 Y, #6518 is G54 Z.

[Marc Davis]

Thanks, I didn't have the manual in front of me when I wrote the mail. I was trying to change #6516 not #6513. Anyway, I can just use G10 to change it until I figure out what I'm doing wrong.

Marc

[dcoupar]

Thanks, I didn't have the manual in front of me when I wrote the mail. I was trying to change #6516 not #6513. Anyway, I can just use G10 to change it until I figure out what I'm doing wrong.

Marc

Here's the applicable page from the MX3 Operator's manual on Displaying and Writing Work Offset (4.3.5.2). Is this the way you are doing it?