G59 P?????

So, figured out that work offsets are my ticket on a multi-part fixture I'm working on. Figured it out how to setting it all up... well okay that may be a stretch..... In Fusion 360, I have my OP setups with G55, G56, G57, G58, G59 set (however I have to manually go in post edit and fix the G55-G59 settings - it wants to post out G59 P55, G59 P56 and so on). On the machine I go into the MDI line put in G55 - probe my part for zero, MDI - G56 - probe my part for zero, MDI - G57 - probe my part for zero, MDI - G58 - probe my part for zero, MDI - G59 - probe my part for zero. All good up to this point.

Background: Each OP uses the same tool, however at each WCS there is a different operation being done. In this case I have 8 total operations to complete the part.

So has got me wondering how do I set up for much larger setups? As in this case I have 8 operations. G54 thru G59 gives me WCS for 6 operations. How do I go into probe the part for G59 P7 & P8? If I go into the MDI line and put in G59 P7 I get an error.

Let me know if I've left something off in my explanation.

PathPilot 1.9.7
Fusion 360

Thanks,
Awall

Looks like I might have found some additional info under the PP offsets page under the work tab. Looks like it uses G59.1, G59.2 and G59.3. Interesting thing is that it will not let me setup above G59.3......

So now I wonder is there a way to set that up in Fusion to post that way vs having to manually edit all the WCS.....

Here is the code I use in the fusion post to get the correct work offsets.

You can search for G59 and look to match the code.


// wcs
if (insertToolCall && properties.forceWorkOffset) { // force work offset when changing tool
currentWorkOffset = undefined;
}
var workOffset = currentSection.workOffset;
if (workOffset == 0) {
warningOnce(localize("Work offset has not been specified. Using G54 as WCS."), WARNING_WORK_OFFSET);
workOffset = 1;
}
if (workOffset > 0) {
if (workOffset > 6) {
var p = workOffset; // 1->... // G59 P1 is the same as G54 and so on
if (p > 9) { // Was P > 254 - Changed for Tormach PathPilot Limits
error(localize("Work offset out of range. Tormach PathPilot Supports G54-G59, G59.1, G59.2, G59.3"));
} else {
if (workOffset != currentWorkOffset) {
p=p-6; // Added for Tormach G59 Limits
writeBlock(gFormat.format(59)+"." + p); // G59 P - Was writeBlock(gFormat.format(59), "P" + p); Modified C.Byrd
currentWorkOffset = workOffset;
}
}
} else {
if (workOffset != currentWorkOffset) {
writeBlock(gFormat.format(53 + workOffset)); // G54->G59
currentWorkOffset = workOffset;
}
}
}

[QUOTE=cbyrd;2013242]Here is the code I use in the fusion post to get the correct work offsets.

You can search for G59 and look to match the code./QUOTE]

Hey cbyrd,

Thanks for the info. So, looking at this, if I have a fixture that has more than 9 WCS I'm kind of screwed.....? G59.4 sends an error. Why would they not allow all 254 possibilities?

I would argue that, with EXTREMELY rare and complex exceptions, if you can't make do with plain old G54-G59, you are doing something seriously wrong.... I have NEVER had to go beyond those 6 fixtures, and the only times I've ever used them all (perhaps twice in 10 years), was because I was working with six vises on my machine, to make three each of two different parts in a single setup...

Regards,
Ray L.

Quote:

---

Originally Posted by SCzEngrgGroup

I would argue that, with EXTREMELY rare and complex exceptions, if you can't make do with plain old G54-G59, you are doing something seriously wrong.... I have NEVER had to go beyond those 6 fixtures, and the only times I've ever used them all (perhaps twice in 10 years), was because I was working with six vises on my machine, to make three each of two different parts in a single setup...

Regards,
Ray L.

---

I would agree, however one of the advantages of the CarveSmart jaws is to have multiple quick change fixtures (say each fixture has 4 different ops per fixture). I could then go in and set/store work offsets G59 P200, P201, P202 and P204 for jaw set #1. Next week, when I run that job again, all my work offsets are stored and can be recalled without having to probe the parts..... unless I overwrite them.

Does that make sense....

Thanks for the input.

Quote:

---

Originally Posted by smokediver576

I would agree, however one of the advantages of the CarveSmart jaws is to have multiple quick change fixtures (say each fixture has 4 different ops per fixture). I could then go in and set/store work offsets G59 P200, P201, P202 and P204 for jaw set #1. Next week, when I run that job again, all my work offsets are stored and can be recalled without having to probe the parts..... unless I overwrite them.

Does that make sense....

Thanks for the input.

---

That approach simply does not scale. No matter how many fixtures you have (and it is always a very limited number), you'll eventually run out. I'm pretty sure LinuxCNC supports only G54-G59, G59.1, G59.2 and G59.3. That is a hard limit, that you cannot change without modifying LinuxCNC itself, and you'd then have to modify PathPilot as well.

Instead, simply write down the offsets for a particular setup, and re-enter them manually next time you need that fixture. No probing needed - Go to machine coordinates display, select the desired fixture, move to the fixture offset, zero the axes, and you're done - takes seconds.

Regards,
Ray L.

Quote:

---

Originally Posted by SCzEngrgGroup

That approach simply does not scale. No matter how many fixtures you have (and it is always a very limited number), you'll eventually run out. I'm pretty sure LinuxCNC supports only G54-G59, G59.1, G59.2 and G59.3. That is a hard limit, that you cannot change without modifying LinuxCNC itself, and you'd then have to modify PathPilot as well.

Instead, simply write down the offsets for a particular setup, and re-enter them manually next time you need that fixture. No probing needed - Go to machine coordinates display, select the desired fixture, move to the fixture offset, zero the axes, and you're done - takes seconds.

Regards,
Ray L.

---

Hey Ray,

Yep, but this assumes one has made their fixture correctly. My issue has been that where I dialed the part in is not exactly where the part is in reality. I tried moving the parts around in the model to adjust but it got real muddy when trying to adjust 9 parts.

My original fixtures had one XYZ WCS registration box and everything was supposed to register off of that. However I kept pulling my hair out until I figured out G55 and so on.

Still learning! Thanks for the G59.1 thru .3 info. That makes sense.

As SCZ stated, the G59.3 is the limit of Pathpilot. I am not sure of the Linuxcnc limit, but it makes sense.

I always leave one of my setups (G55) as my offset for my ETS.

If you're really determined to do it that way, I suggest you read up on G10, which lets you set the offsets in g-code. That would allow you to code the fixture offsets directly into the g-code. If the issue is fixtures that are not precisely where they are supposed to be, you can also deal with that using G92 (and I think maybe G52), to "fudge" the offsets as the program runs.

Regards,
Ray L.

This is one of the reasons I have not switched to PP. I have dedicated fixtures that hold up to 12 parts. I set it up so that I define a different work offset for each part, G59P11...22. In SprutCam I program only 1 part. I manually edit the Gcode to add a line number and a few variable assignments after each tool change and just before the next tool change add a call for a custom macro (M253) and an M98P and another line number. The program will run the first part then increment the work offset (G59P11 to G59P12), loop back and run the next part. At the end of the last part it exits the loop, changes tool and runs the next operation on part#1 (G59P11). If I have an issue with a fixture location, like stripping out a hole for the mighty bite clamp, I just don't define an offset at that location. If I only have material for 9 parts instead of 12 I just tell it to do only 9 parts (one of variables assigned at the beginning). Has worked well for me.
If there is a way to do something similar in PP it would make switching more attractive, I'll have to look into the G10 command. I would still have to re-write a hundred or so custom macros. Not an easy switch over.

Is G92 stable in LinuxCNC? The Mach3 manual sternly warns against using it. Years ago I ignored that advice and it demonstrated why you shouldn't use it.:mad: Cost me a part I had 12 hours into and $200 in material.

Quote:

---

Originally Posted by IMT

This is one of the reasons I have not switched to PP. I have dedicated fixtures that hold up to 12 parts. I set it up so that I define a different work offset for each part, G59P11...22. In SprutCam I program only 1 part. I manually edit the Gcode to add a line number and a few variable assignments after each tool change and just before the next tool change add a call for a custom macro (M253) and an M98P and another line number. The program will run the first part then increment the work offset (G59P11 to G59P12), loop back and run the next part. At the end of the last part it exits the loop, changes tool and runs the next operation on part#1 (G59P11). If I have an issue with a fixture location, like stripping out a hole for the mighty bite clamp, I just don't define an offset at that location. If I only have material for 9 parts instead of 12 I just tell it to do only 9 parts (one of variables assigned at the beginning). Has worked well for me.
If there is a way to do something similar in PP it would make switching more attractive, I'll have to look into the G10 command. I would still have to re-write a hundred or so custom macros. Not an easy switch over.

Is G92 stable in LinuxCNC? The Mach3 manual sternly warns against using it. Years ago I ignored that advice and it demonstrated why you shouldn't use it.:mad: Cost me a part I had 12 hours into and $200 in material.

---

Doesn't your CAM provide some way to do patterning? I can program a single part in HSMWorks/HSMXpress, then repeat that code at any number of other locations in a 2D linear or radial array, to cut as many of that part as I want, using only a single "fixture". If the parts are not located on a consistent pattern, I can just create an assembly in CAD with the parts located wherever they need to be, then do the CAM based on that assembly. This, again, let's me use only a single fixture to make parts even if the holding fixture has some/all the parts mis-positioned.

I never, never, EVER have hand-edit the g-code....

Regards,
Ray L.

Quote:

---

Originally Posted by SCzEngrgGroup

If you're really determined to do it that way, I suggest you read up on G10, which lets you set the offsets in g-code. That would allow you to code the fixture offsets directly into the g-code. If the issue is fixtures that are not precisely where they are supposed to be, you can also deal with that using G92 (and I think maybe G52), to "fudge" the offsets as the program runs.

Regards,
Ray L.

---

I really like this G10 idea. This would allow you to dedicate one offset as your "Carvesmart" offset and allow the individual programs to dictate the position and overwrite the offset, rather than tying up all your offsets which are limited. If you run a lot of parts, from my experience, it is inevitable that you accidentally re-zero an offset that you didn't mean to, and in my opinion it would be more prone to a crash. On the downside, once you take of that vise for plate work or whatever your hit, unless you have a tool plate or something you can come back to. Just my thoughts.

Pete

Quote:

---

Originally Posted by SCzEngrgGroup

Doesn't your CAM provide some way to do patterning? ....
I never, never, EVER have hand-edit the g-code....

Regards,
Ray L.

---

Yes it does. However that isn't the point. I want to be able to run 1 to 12 parts from any of the fixture locations WITHOUT going back to the CAM. I have no problem hand editing. I wrote programs that way for years.

Replied before seeing the last page. I thought I could delete this but I guess not.

I probe the top of the upper-left corner of my CarveSmart master jaw - its on the 5" Tormach vise, so the upper left corner pokes out of the vise making it easy to probe all axis. This is my "zero" location X/Y/Z.

In SprutCam, I model the master jaws as fixtures, and locate the parts in the soft jaws (this puts them roughly at X0.5, Y-2, Z something). Then every program that uses CarveSmart jaws just needs one probe point to get the zero and all part offsets are correct. Swapping the soft jaws does not require re-probing, since the master jaw doesn't move.

If you use tall soft jaws and plane them down each time for a new part, you could keep the X/Y on the master jaw, but re-probe the Z for the new jaw height.

--Bryan