help with gcodes

[turmite]

I am still stumped with my G90 code. I have written G91 code for so long it is hard for me to grasp this thing.

My machine is set up to touch a switch to set the tool length and the
retract to a point that is then reset to x0y0z0. I am carving rifle
stocks using a 4th axis. The starting point of all my programs for
the stocks once centered x and y over the workpiece is z-1.541"

My cam program writes the gcode for a ball nose cutter for the center
of the radius. Using the switch to set the tool is from the tip of
the ball. I use a .750" diam. cutter for all my carving and inletting
for all the round actions and what part of the barrel channel I can
get with it.

My question is: How do I write my programs? Do I have to redraw
everything with the xyz beginning cordinates and then change the
geometry fo using the tip of the tool, or can I do a Gz offset, which
I have tried and it didn't work, but that may have been because I
didn't get it right too.

It would be so easy for me to fix this in G91 by adding a G01z-.375
at the beginning and a .375 at the end. I can't use the G91 because
the cam program introduces serious step losses when in the 91 mode.
Mach2 controller (I have posted this there also)


Mike

[cadcam]

What are you using for cam?

So are you saying that your system will not comp for the tip of the tool only the center?

[mtlmnchr]

there must be a parameter to tell the machine how far to retract , correct ? can you adjust this value to compensate for the center of the tool nose ? (Kind of like a tool lentgh compensation offset)

As I understand this is only affecting your Z axis ? or did I miss something ?

another solution might be to shift your geometry in your model to adjust so you don't have to adjust your parameter.

[wjbzone]

Mike,
I program the center of the ball in my cad system also.
If I teach to tool length at the end of the ball, it cuts air. (runs too high) It needs to be lowered by the ball radius. Just offset your Z.

When I set my tool length I always remember the rule "Bigger number (in the G50 Z offset) the smaller my part gets".

Bill

[turmite]

Thanks for the replies guys.

cadcam let's just say I can't afford one like you sell, and they advertize here on the Zone and their logo is a small type cat!

mtlmnchr I have tried everything I know. Now that is not to say I don't know how to use the program properly. I am self taught and that may bell the problem. I have tried to redraw/reposition the geometry but when the program writes the cam it still writes it to the center of the ball and not the tip.

Bill that is what I want to do but I am using Mach2 and am just now learning to use it properly. A good old G91 sure looks good to me right now!

Mike

[mtlmnchr]

how about finding a piece of flat stock that is .375 thk and placing it between the material and the tool when setting the Z ? or is it affecting all the numbers ?

[HuFlungDung]

Mike,

Are you saying you never use a Z tool length offset? That is the obvious place to make the tool height adjustment that you require.

What coordinates do you assign to the machine home position (the place where your tool always starts from)? Is it simply X0 Y0 Z0?

If this were the case, you might be able to change those coordinates by inputting a line like
G92 X0 Y0 Z.375

In the absolute coordinate system, this (should) tells your controller that the home position of the tool is not Z0, but rather Z.375 When it makes an absolute move to Z0, it will move downwards an incremental distance of Z-.375. As you know, in incremental programming, a movement command of G91 Z0 does nothing, but in the absolute system, G90 Z0 will cause a movement from wherever the tool is located now, to the Z0 plane.

This G92 line should be near the beginning of your programs to define the tool position relative to the X0 Y0 Z0 of your part. As a warning, G92 can cause a new work home to be defined at any time, so you must never use more than one instance of G92 (until you know what you are doing). A second warning, is you must be absolutely certain to return to home every time you abort your current move or the program you are running. Imagine stopping at the far end of the part, resetting the program and it starts up again and thinks "ahha, this is the new G92 home position way over here!" Not pretty results.

Then there is the preferred method of using a G54 to G59 work offset which is safer than the G92. But, you can ask about that if you want to know.

Using absolute coordinates is not really the problem here, although I can see how you are stuck if you think there is no other way to make the adjustment

[turmite]

mtlmchr that will change only the first move in absolute. After that the code still reads the absolute position from the home 0 position.

Hu let me go inot just a little detail here and maybe you can help.

I made a z axis reference switch so I could set the bottom of all my bits with a macro call tool set. Aftering zeroing the machine I hit the tool set button (icon) and the z axis moves down till it touches the switch. It then retracts ?? from the switch and rezero's itself there. The starting position of all my rifle stocks are a known absolute position above my a axis and they are real close to the following.

x27.4527y108.2754z-1.451

This is the first move in the program as I have positioned my drawing with that point above the a axis and above the part by 4.5 in. This gives me a safe z that in case I need to rotate the part I can do so without having to change any other settings. Would the following work?

1G0x27.???y108.???z-1.451
G92 z-.375
rest of the program?????????????????????????
G whatever to cancel the G92 and I think it is G92.1 but I can find that.
M30

Mike

[HuFlungDung]

Mike,

No, you should not make any programmed machine movements before you execute the G92.

The G92 position should be determined before beginning the program. You typically would define a reference point on your work, that you call X0Y0Z0. You jog from your tool home to this position (use an edgefinder perhaps) and when you are at this position, then you note how far you have moved. You might have to invert the signs from plus to minus, but basically, these distances define the values for your G92 home.

Perhaps one safe way to do this, is to not write the G92 line into your porgram. Rather, execute it in mdi mode. This should set your machine and reset the displays.

When using a horizontal A axis ( if I am picturing this correctly), the centerline height of your A axis should (most conveniently) be reckoned to be Z0 in absolute position. You could reference it to some other cylinder height if you wanted to.

Your part should be positioned with its axis on the A centerline of the workpiece, too, both in your cadcam program (before you generate code), and on your machine.

But for the sake of explanation, suppose your Master Tool is at home position. Suppose also, that this Master Tool uses no Z tool length offset. If you measure (by jogging) the amount of movement from the tool home position to the A axis centerline, this amount would be your G92 Z home amount. Suppose the distance was 4 inches. It might read -4.0 on your display because you have jogged downwards from zero.

So, return the tool to home and input
G92 Z4.0
G90 G00 Z0

The first line will describe the tool home Z position relative to your A axis. It should reset your machine displays to this value : Z4.
The second line will cause a rapid movement to bring the tool tip to the A axis centerline height. This movement is just a test to see if that actually happens.

There is no method of cancelling a G92. If you want to use G54 to G59 work offsets, there is a cancel code for that, which is G53. Would you rather use a work offset?

[turmite]

Thanks Hu. For once someone explained it in a way that I can understand what was meant. I can see there is going to be no real easy solution for my problem other than possiblyu writting some macros.
Thank you very much for your help. I'm sure I'll be calling again!

Mike