How do I set the tool table?

More
09 Oct 2018 20:00 - 09 Oct 2018 20:02 #118604 by Einar
I haven't used the lathe for months. Primarily because after changing a tool it takes me a couple of days to get the tool table working properly. The procedure have been to use the Touch off function in Axis to get me somewhat Close. Then go in and fine tune it by calculating offsets to whatever was there. But this can easily take many hours With 8 Tools!

So I thought I would try overriding tool 1 to X=0, Z=0 as suggested: forum.linuxcnc.org/26-turning/26991-conv...-250b?start=40#74100 . I did that by editing the tool table, then saving it.

Then I brought tool 1 to the face of my part and did Touch off G54 Z=0. Then X to the periphery of a 12.5mm rod and Touch off G54 X=12.5.
After that did a M6T3G43 to bring in a threading tool. Jogged it to point at the face of my part and Touch off Tool table Z=0. Then touched the periphery of my part and entered 12.5.
After this the DRO's showed silly numbers! I include a screenshot in case there is a Clue in there that I don't know I should mention. Other than tool 1 and 3 the tool table shows "old" numbers not touched in this attempt.

It may be a clue that the numbers seems pretty Close to the offset from the home position.

I really hope I can get somewhere With this. As it is the lathe just sits there occupying space. After trying to do something with it I am close to needing psycotherapy.
Attachments:
Last edit: 09 Oct 2018 20:02 by Einar.
More
10 Oct 2018 13:22 #118636 by andypugh

Einar wrote: After that did a M6T3G43 to bring in a threading tool. Jogged it to point at the face of my part and Touch off Tool table Z=0. Then touched the periphery of my part and entered 12.5.
After this the DRO's showed silly numbers!


That's odd.

You _might_ need another G43 after the touch-off. (You do with Touchy).

I assume that the DRO is set to show work coordinates?

You need to enter a diameter if the lathe is in Diameter mode, and a Radius if the lathe is in Radius mode (both when touching off T1 into G54 and when touching-off the tool table.)

G10 L1 P1 X0 Z0 will set the tool-1 tool-table to zero, that's easier than editing the tool table.
More
10 Oct 2018 19:22 #118649 by Einar
Replied by Einar on topic How do I set the tool table?
I tried adding G43 after Touch off. It did not seem to make any difference.
The lathe is in diameter mode. I find that most intuitive.

It seems to me that what goes into the tool table when I Touch off Tool table is an offset from machine home position.

Could it be that my version of LinuxCNC (2.6.0~pre) have a bug that have been driving me mad?
I do not know how to find and traverse the version list to see if this is a bug that have been fixed.
And I never found this to be working as expected.
It seems to me very few are using LinuxCNC for a lathe, so lathe specific bugs may go unnoticed for a while I think.

Just now I have too many other items (cars, house, ...) that needs attention to start a new install.
But if it is a known bug I will at least just stop trying until I can do a new install.
More
10 Oct 2018 19:42 #118651 by andypugh
No, I have been using LinuxCNC with a lathe since 2.4 and it has always worked as-expected.

Later versions do at least have separate buttons for tool touch-off and coordinate-system touch-off.

When you touch-off, whether to G54 or the tool-table, the DRO should show the number you typed.

One thing that might change this is if you have "tool touch-off to fixture" set in the machine menu.

Also check that you are displaying commanded position and relative position in the View menu, just to keep things simple.
The following user(s) said Thank You: Einar
More
11 Oct 2018 16:16 #118673 by Einar
Replied by Einar on topic How do I set the tool table?

andypugh wrote: One thing that might change this is if you have "tool touch-off to fixture" set in the machine menu.

And that is what it was set to!
Now corrected and everything works just as expected.
Thank you!!!!!
More
27 Nov 2018 15:54 #121477 by Cayenne
Sounds like my problem!
If my machine has no limit or home switches and no tool changer why do we need to home the axis?
If the stock, part, toolpaths, retracts, etc. are all within the machine envelope soft limits are not required, right? If I zero my Z and set the X by touching off to part I should not need any tool length offsets, correct? I am using a manual quick change tool post.
what would a tool length offset be relative to??? as the tip of the tool is an arbitrary point in space. I do understand it could be relative to a different tool tip after this new tool is touched off to the same surfaces as the original tool.
A couple of versions back I would do just this! touch off the tool and start making parts now it's just mathematical insanity where nothing is reproducible. even the inputs for touchoff, and tool touchoff seem to randomly prefer radius or diameter. Can someone please point me to a current startup work flow for turning?
More
29 Nov 2018 15:47 #121593 by andypugh

Cayenne wrote: Sounds like my problem!
If my machine has no limit or home switches and no tool changer why do we need to home the axis?


It is very useful to allow restarting of jobs, and also means that the system can know that it can machine the part without hitting the end stops. It also means that the software can avoid ever hitting the end stops.

I have no idea why folk are so resistant to fitting a few extra switches and wires.

But, if you really object to home switches then there is an INI file option ( [TRAJ]NO_FORCE_HOMING ) that means that homing is not enforced. There is also the option to record the shut-down position too. ([TRAJ]POSITION_FILE)

I am using a manual quick change tool post.
what would a tool length offset be relative to???

If this is a lathe, then typically the tool length offset of any tool is relative to the length of a probe or another tool. All my tool lengths are relative to my Tool 1 (turning and facing) tool. I jog to the material end, touch-off G54 to zero, and take a facing cut at Z=0 with tool 1. Then take a test cut to a diameter with the same tool and set that as the G54 X offset. Then I can change tools to (for example) a threading tool and the diameter and length are correct.
Actually, I don't do that second part very often, as I have my lathe set up with single-turn absolute resolvers and a bit of cleverness with the POSITION_FILE means that my lathe always knows exactly (to the micron) where it is at power-up)

now it's just mathematical insanity where nothing is reproducible. even the inputs for touchoff, and tool touchoff seem to randomly prefer radius or diameter. Can someone please point me to a current startup work flow for turning?


Whether radius or diameter is set depends on whether the machine is in G7 or G8 mode. I think it starts up in radius mode. A STARTUP_G_CODE can change this.

There shouldn't be any mathematical insanity. Perhaps you are touching-off tools when you should be touching-off coordinate systems? (and possibly your system, too, is set to "touch off to fixture"?
More
30 Nov 2018 14:18 #121633 by Cayenne
Thank you very much for this concise info!
Yes, "Lathe" that is why i posted in this sub forum.
"touch off to fixture" is not in effect !
LCNC is set to radius mode.
When I first start LinuxCNC the "touch off" obeys the radius mode input.
The "tool touch off" wants diameter inputs and later, it wants radius inputs (bug?) maybe I'm not understanding things. and yes, operator error is a strong possibility!
So if I use tool for tool I should only need "touch off" correct?
How do we zero out all offsets?? because ounce I enter the wrong tool g54 offset, no matter what I do i can never zero out the g54 in order to start over.
I have been using F360 for toolpaths, which compensates for tool tip radi (i believe) so should i enter a tool tip radius in LCNC tool table? Again, Thank You!
More
30 Nov 2018 14:30 #121634 by andypugh

Cayenne wrote: When I first start LinuxCNC the "touch off" obeys the radius mode input.
The "tool touch off" wants diameter inputs and later, it wants radius inputs (bug?) maybe I'm not understanding things.


If the machine is in G7 / Diameter mode then the number you type in will become the current diameter.
If the machine is in G8 / Radius mode then the number you type in will become the current radius.
You can experiment with this, switch between G7 and G8 using MDI and try touching-off your G54 coordinates.
(This is rather more obvious in Touchy as that permanently displays both radius and diameter.) And I quite often find it not doing what I expect, but that is because the lathe has been left in an unexpected mode (I work nearly always in diameter)


How do we zero out all offsets?? because ounce I enter the wrong tool g54 offset, no matter what I do i can never zero out the g54 in order to start over.


"tool G54 offset" is a phrase that makes no sense, and if that is what you really meant then this might explain part of the problem.
In any case MDI
G10 L1 P10 X0 Z0 R0 I0 J0 Q0
will zero-out all tool-table data for tool 10.
G10 L2 P0 X0 Z0
will zero out the work offsets for the current coordinate system. Use P1 for G54, and so on.
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g10-l1


I have been using F360 for toolpaths, which compensates for tool tip radi (i believe) so should i enter a tool tip radius in LCNC tool table?

The radius in the tool table doesn't matter unless G41 / G42 are active. and Fusion CAM does not use those.
Moderators: piasdom
Time to create page: 0.097 seconds
Powered by Kunena Forum