A couple of Centurion V programming questions

[Brian L]

My machine is up and running, still have a lot to sort out, but I was/am making this adapter to hold the monitor arm. In the process of programming and running a couple of operations I ran into to some things that brought up questions....

First, when you home the machine, then go find your work 0,0, using an edge finder or whatever, then you hit Floating X and Y, to zero out your work coordinates. Now, I've been writing those numbers down, say X-15.510 Y-8.712 is my part zero from home. If I want to come back the next day, or have to rehome the machine... the previous floating zero's are lost, correct? I have to type into MDI G01 X-15.510 Y-8.712, input and start to move to that position.

Kind of along that same vein, past brands of machines I've run have a position page that shows absolute machine home, part home , distance to go and such. This way if I'm jockeying around to get my part zero, zero, I can always go to that page, find out how far I actually am from home and get those numbers. As it sits now, I'd have to take the numbers I wrote down, add/subtract in any adjustments and get new numbers. If I try homing to see what the numbers from part home to machine home is/are, it zero's out and I am lost and get to start all over again.

I was cutting a partial arc.... still a bit fuzzy on the conversational, so rather than take a chance, I just typed in the g-code. Ran into an error with my code and am wondering if/what the issue is.... ok, part has a pivot hole that is center of the arc, 3.5" in the Y minus I wanted to start my arc and go 18º CW (so from about 6 o'clock to 7 o'clock). Code looked like this:

G00 X0 Y-3.5 (center of the beginning hole)
G01 Z-.5 F15 (go down)
G02 X-1.081 Y-3.33 J3.5 (cut arc to the left)

This wouldn't run (the numbers above are a guess, I have the papers in the shop with the exact numbers). I double checked my end points, they are right, do you have to have an I and J, even though the I value was zero, because it's a partial arc? I use just one or the other for full circles all the time, but suspected that because it's a partial arc I needed both. Solved it by using R instead of I J, but that's kind of a half ass way of getting around it.

Enough questions for this post... for now...

[ZZZZ]

Get into Level 3, Go to the MISC parms, cursor down to "Use FLZ instead of G54" and change it to "NO". Now the G54 Work Coordinate offset values will remain active until you change them. You can power down, come back tomorrow, power up, home, and MDI back to X0Y0 and get back to the same point. You can also use all 6 Work Coordinates, G54 - G59 by changing the active WC system in MDI. Power-up defaults to G54. You can see the WC offsets by going to F7-Parms, F2-Coord and arrowing down

I think you should be able to program your arcs using Incremental Centers (X,Y,I,J), Absolute Centers (X,Y R,XC,YC), Polar (AA,AB), or Radius only (R, X,Y). I tried a partial arc without both I and J and it worked for me.

[Brian L]

Thank you ZZZZ, that makes sense. Is there still no position screen available to tell me where I am in relation to the true machine home though? Or, if I set these parameters, and zeroed out my G54 position, would the machine read say X15.xxxx Y8.xxxx when it homes and I'll know that dimension?

The arc program, I'll go back to it and try it again.... I did find that my end points were off originally, my CAD system had defaulted to rounding to the nearest .001" instead of .0001"... so I was like .0004" off in X and .0003" in Y, so maybe that was the issue. I might not have tried the just J value with the right end point values.... could have changed to R and the right values at the same time.

It might take me a day or two, I pulled the whole control panel off the mill last night. I have to install the arm extension, pull the wiring through it. I found a keyboard adapter I'm extending off the board and to a panel mounted port, so I can attach a keyboard without opening the box. Also fished an ethernet (RJ45) cord from the back of the machine up through the arm and into the control and mounting an ethernet port on the console too. That way I can hook my laptop/shop computer to it directly to upload/download or DNC if I ever get to that point.

It's getting exciting putting things back together instead of tearing them apart.....

[ZZZZ]

There isn't a specific screen for that purpose. When using the Work Coordinates (G54-G59) rather than Floating Zero (G92), you could go to MDI, give it an unused WC such as G59, and the display would show the position from Home position as you would have no offsets active. Then change back to your current WC and the display will show your current position.

The control defaults to G54 at power-up, so after Homing, the display shows your position using the stored offsets from Home. You can go to F7-Parms F2 Coords, arrow down to G54 and see the same numbers as the display with the signs reversed.

[Brian L]

I got my control powered back up today too late to try any of this, but it sounds like (if I understand this correctly) I could indicate in wherever part 0,0 is, call G59 and it will give the opposite values of part zero to home position, correct? If so, that'll work.... too many times I get jogging around and change work zero and then wouldn't want to get confused.

[ZZZZ]

Brian, go change the MISC parameter as I discussed in post #2.

Then go to HDW, pick-up your part edge, sweep the hole, whatever. When you are in position, with the X axis active, press the G54-X button, when you have the Y axis active, press the G54-Y button.

The DRO will change to zero when you press the button and the values will be entered in the G54 offset fields in the parameters table.

The Z-Tool button will set the tool length offset and put that value in the Tool Table.

[chipsinpan]

from the main screen , go to PARAM then COORD.
You can then scroll down to G54 thru G59 and you will see the distance from home zero to wherever you zeroed the selected work coordinate .

I usually save G59 as my part change position .
I will HDW the table to a place where it is convienent to swing the vise handle , and clear tools then I call this G59 and zero XY
At the end of each program I just write G59 X0 Y0
Z is not dependant on work coordinates , it is just the tool height .

Using the G59 the way I do is not an accepted practice , just my personal choice .

The correct way , is to move to the position you want , then go to PARAM/ COORD , and write down the coord from home zero (X Y) fro the LAST WORK COORD CALLED then enter these values on the last program block where is says XY home relative

[Brian L]

New question that has cropped up.... wrote a program to make some softjaws for my Kurt vise. In the process of milling and putting the bolt holes in, I want to helical mill into the hole and counterbore for the 1/2" bolt head.... basically a .760 diameter by .530 deep. So I moved off center of my hole by .130" (using a 1/2" endmill), started .050" above the part and wanted to helical cut into the part .058" per revolution, so I make 10 loops to my depth.

I thought that line would be like this, in incremental, by the way:

G03 I-.13 Z-.058 L10 (that giving me 10 loops)

Well, I got one loop, and then it moved on to the next line. I fixed it by just adding ten lines of code, the same G03 I-.13 Z-.058 ten times in a row. Does the L command not make the line loop? Reading about subs and looping in the manual it would appear too, but it didn't seem to work as expected.

[ZZZZ]

The looping technique allows for looping another program from inside the main program.

M98 PXXXX LXXX
PXXXX = subprogram number
LXXX = number of times the subprogram is to be repeated

Example: M98 P0002 L5 calls program O0002 5 times

OR

You can have a sub call inside the program:

GOSUB 9999 L10
G90 (back into absolute)
M30 (end program)
N9999 (or some unused line number)
G03 I-.13 Z-.058
RETURN

[Brian L]

OK, so you can't loop just a line without turning it into a subprogram and then calling that multiple times? Or having the sub actually part of the main and using GOSUB, then RETURN....

It's been a lot of years, but I sure seem to remember doing thread milling with the Fanucs and calling the circle line with an L for the number of revolutions. Most of the time we used specific pitch thread hobs, but for that occasional oddball pitch, we would make however many circles it took to get up and out of the hole.

Thanks for the tip on the GOSUB, makes it nice to have all the lines in one program rather than having the main and multiple subroutines, which is what I did today. I need to fine tune where I put my M05's and such.... had about half the program where the spindle started back up after my M00 (stopping to flip the parts in the vise) and the other half it stopped and stayed stopped.

Do you need an M03 SXXXX call on a line separate, and alternatively, do you need an M03 and have to have the S call, or will it just revert to last speed if you just use M03?

[ZZZZ]

Because the spindle speed is modal, the M3/M4 command by itself will start the spindle.

[Brian L]

That's what I thought, all I would need is an M03. Now, does any M code have to be on a separate line? Can I have G00/G01 lines and throw in M03/05 anywhere I want? Some control variations I've run over the years were picky about how many M codes were used in one line and some M codes of one group, couldn't be mixed with others.

On that same thought, when placing an m code on a line, does order effect how they are carried out, i.e. if I put a spindle start on a line and it's before a rapid move, does it turn the spindle on and then move, and if I was to put the move and then the m code, does it start to move first and then turn the spindle on... or is anything on one line done simultaneously?