[saabaero]

In MACH 3 I used to be able to use my probe to find the coordinates of the center of a hole but in PathPilot I seem to only have the option of setting the center of a hole to the new zero point. I just want the coordinates. Has anyone figured out how to do this without writing a program from scratch?

[CountrySmith]

Can you change to a different coordinate offset, e.g. G55, G56, etc. and probe and then switch back to the original offset?

[GenInt]

CountrySmith has the correct answer. Specifically, if I wanted to find the center of a bore relative to G54, I would probe it using a different offset, (for instance G55. After the probe finds the center and zeros out G55, without moving anything, switch back over to G54, and the X,Y coordinates shown will be the center of the bore relative to G54. Later, provided I haven't re-probed G55, anytime I send G55 to X0, Y0, and then switch back to G54, I will get the same result - or at least within a couple of 10 thousands.

The other way is to stay in G54 and on the first probe screen you have "FIND X+, FIND X-, FIND Y+, FIND Y-" buttons. Bring your probe down to roughly center, (doesn't have to be exact if it's a circular bore). Do each of the "FIND" buttons. You can then calculate the center of the bore away from G54 X0, Y0, but you don't need to do any calculations if you use the method above.

[saabaero]

Thanks guys! I hadn't thought of switching offsets but that's a great idea. I'm just surprised that Tormach didn't include a button for such a common task as finding the coordinates of hole centers. I wonder how hard it would be to modify the conversational programs.

[GenInt]

I'd say that it would be pretty simple if one had the PathPilot source code. Basically, I think you would just add another button that does the exact same thing as the one that's there now except you would just delete the section of code that resets the system variables for the current X,Y coordinates to 0,0.

[dneisler]

ounds like a great suggestion for someone to add over at the tormach pathpilot website.

BTW... I was told 1.9.6 should release next week.

[SwampDonkey]

How would this be used in practice? Ive never used G54 or G55.

[saabaero]

How would this be used in practice? Ive never used G54 or G55.

Let me start by explaining the reason for G54, G55, G56... offsets for those that might not know.

Suppose you had a part that you want to make 3 of that are spaced 4 inches apart using the same piece of stock. You can just set your G54 (default work offset system) origin at 0,0,0 and then move 4 inches in the +X direction, activate G55 work offset coordinate system, and set that point to zero. Lastly you would then move 4 inches again in the +X , activate G56 and then set that point to zero. Then you can run the same program and just alternate between activating G54, G55 and G56 work offsets.

With that in mind if you want to find the relationship of a hole center with respect to the part origin (e.g. bottom left corner) you could activate the G54 work offset and set X0, Y0 to the part lower left corner. Next you would activate G55 as the current work offset coordinate system and probe to set the center of the hole to zero. Without moving the machine you would then switch back to the G54 origin and the display would show the current (hole center) location with respect to G54 (part lower left corner). Since PathPilot wants to set the hole center that it finds to zero the main purpose is to switch to another work offset system so the lower left corner origin doesn't get overwritten. Any work offset G56, G57, and etc. would work fine for this purpose.

MACH 3 was simpler than PathPilot in that you could probe the center of a hole and display those coordinates without setting the hole center to zero. In PathPilot you can only probe to set the center of the hole to zero.

Hope that helps explain things a little better.

Oh, and one other thing I don't like about PathPilot... That is that there doesn't seem to be any way to manually edit the work offset table by just changing values in the table. To set the offsets one has to physically move the machine to the new location, activate the new work offset system and set 0,0,0.

[vmax549]

I beleive that the code to find a center of circle is still in the Lcnc manual , Copy the code and run the routine in Path Pilot. Easy peasy.

(;-) TP

[SwampDonkey]

Let me start by explaining the reason for G54, G55, G56... offsets for those that might not know.

Suppose you had a part that you want to make 3 of that are spaced 4 inches apart using the same piece of stock. You can just set your G54 (default work offset system) origin at 0,0,0 and then move 4 inches in the +X direction, activate G55 work offset coordinate system, and set that point to zero. Lastly you would then move 4 inches again in the +X , activate G56 and then set that point to zero. Then you can run the same program and just alternate between activating G54, G55 and G56 work offsets.

With that in mind if you want to find the relationship of a hole center with respect to the part origin (e.g. bottom left corner) you could activate the G54 work offset and set X0, Y0 to the part lower left corner. Next you would activate G55 as the current work offset coordinate system and probe to set the center of the hole to zero. Without moving the machine you would then switch back to the G54 origin and the display would show the current (hole center) location with respect to G54 (part lower left corner). Since PathPilot wants to set the hole center that it finds to zero the main purpose is to switch to another work offset system so the lower left corner origin doesn't get overwritten. Any work offset G56, G57, and etc. would work fine for this purpose.

MACH 3 was simpler than PathPilot in that you could probe the center of a hole and display those coordinates without setting the hole center to zero. In PathPilot you can only probe to set the center of the hole to zero.

Hope that helps explain things a little better.

Oh, and one other thing I don't like about PathPilot... That is that there doesn't seem to be any way to manually edit the work offset table by just changing values in the table. To set the offsets one has to physically move the machine to the new location, activate the new work offset system and set 0,0,0.

Ah. So its all about having more than one 0,0,0 start point. Ive made multiple parts in a fixture but did it the hard way I guess. Im assuming you could make 3 totally different parts with this as well?

[GenInt]

saabaero,
Regarding your post,

"Oh, and one other thing I don't like about PathPilot... That is that there doesn't seem to be any way to manually edit the work offset table by just changing values in the table. To set the offsets one has to physically move the machine to the new location, activate the new work offset system and set 0,0,0."

Maybe I don't understand what you mean, but you can edit the values for any particular work offset by changing the values shown. For example, lets say I'm in G54 at 0,0,0, but I really want G54 0 to be +2.0 in the X direction. My display shows that I'm in G54, and the DRO, (digital readout), box for my X position shows "0.0000". I can just click on that DRO, type "2.0" and hit my enter key. You also don't have to be at X0,Y0,Z0, to do this as you can add or subtract from these values as you wish.

As a side note, I think you might be interested in my posts to the thread "there's got to be a better way" in this forum where I show how you can use one fixed set of Gxx work offsets and one floating set of work offsets that can be manipulated within your G-code using the "G10 L2" command to do things like step & repeat and so forth.

[saabaero]

GenInt,

I know what you are saying about activating the work offset through the MDI and then entering the value in the display. However, I was hoping to not have to activate the work offset in the MDI and then remember to make sure the value I enter in the display is in the opposite direction of where I want the actual offset to be. Normally I just activate the work offset, jog to the location I want the new offset to be and then press zero. It just seemed like it would be easier to be able to go into the work offset table (the tab next to the tool offset table) and then just go down the list, click on a value and changing it. It just seems counterintuitive to me to have a table with values you can click on but can't change. That's kind of opposite to how the tool offsets are changed. But maybe there is still something I'm missing.

As a side note, I think you might be interested in my posts to the thread "there's got to be a better way" in this forum where I show how you can use one fixed set of Gxx work offsets and one floating set of work offsets that can be manipulated within your G-code using the "G10 L2" command to do things like step & repeat and so forth.

Yes, I will check it out! I am always open to learn new tricks. Thanks for the input.