Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: N4NV on January 23, 2019, 10:04:14 AM
-
I have set up my lathe tool table using tool 1 as reference. How can I make an adjustment to tool 1 without having to reset all the other tools?
Vince
-
I don't know the details of how a tool table works so forgive me if this idea isn't practical.
Assign a new tool number to the new position you want for tool 1. Then use the new number instead of tool 1. Tool 1 remains only as the reference for other tools.
-
I have an 8 tool carousel that is electronically linked to Mach, meaning each position is hard wired. I can't fool Mach into thinking tool 1 is anything other than tool 1 (like it can't be tool 9). I also can't have a tool 0 as it is greyed out in the tool screen.
Vince
-
Vince,
Do you use probing to set up / populate the tool table?
Tool 0 info can't be changed in Mach. Tool 0 is not recognized by many programs as a valid tool number.
But, a tool like tool 0 with no offsets, can be used to advantage for measuring when in Machine Coordinates.
I use the master tool concept where tool #1 is the master tool and has no offsets which makes tool zero 0
usefull for setting up tool and work ( ie; you can't screw up the tool table by changing tool #1 offsets which will change the other tool offset.
Have you looked at the G10 L1 command which will change the tools offset?
You can also use "wear" in the tool table to provide for adjustment of a tool.
Also note that you have a master tool and that all the other tools are related to the master tool, but,
also understand that ALL the tools are related to each other. Thus any tool can be used for setup
once the tool table is populated appropriately.
RICH
-
I am aware of the wear in the tool table. I'm not sure how G10 would help me. No I don't use a probe to set up the tool. I put a 1/2" precision pin gage in the headstock and set all the tool offsets from that. Now, each time I am working on a project, I set tool 1 based on the length and width of the stock and the rest of the tools are good to go, correct?
Vince
-
Vince,
1. I have set up my lathe tool table using tool 1 as reference.
How can I make an adjustment to tool 1 without having to reset all the other tools?
You are correct in knowing that if you change tool number #1 offfsets it will affect all the other tool use."All" the tools were originaly touched off to same reference point / surface. One can change all the other tool offsets appropriately based on tool#1 adjustment or physicaly position tool#1 back to where it should be relative to the other tools.
So the easiest way would be to touch off to the the X and Z reference points using one
of the other tools ( their relationships have not changed). Then select tool #1, and move the correct distance, to the same X and Z reference points and reposition tool#1 in the holder. Now repositioning the master tool can be a PITA and that's why I use the equivilent of a cut off tool for the master tool since it has flat sides and a perpendicular front.
I assume you danaged tool#1 which was the master tool. Frankly the master tool should not be used for machining and and it should not have any tool offsets!
2. I put a 1/2" precision pin gage in the headstock and set all the tool offsets from that. Now, each time I am working on a project, I set tool 1 based on the length and width of the stock and the rest of the tools are good to go, correct?
Most programs produce code that is precompensated for lathe tool geometry.
Most generated code will be based on the stock being at some X and Z=0 where the stock centerline is on the lathes center line and the stock face is Z =0. If the tool table is correct, touch off with the master tool#1 to define a work offset (G54 is Mach lathe default) and all should be good to go. From a defined tool change / home postion you can touch off with any of the tools.
I suggest the following if using Mach3 Lathe:
- Use a different screen set than the default Lathe Screen set.
- Use probing for work set up and tool setting.
- Create a custom screen set to satisfy how you work.
FWIW,
I use a simple homemade four surface tool setter which takes care of "ANY" type of lathe tool. A pin is just a PITA and you will make mistakes.The probing and a custom page to set tools just makes ease for the whole process.
RICH
-
I have not damaged tool #1, but I do use it. I only have 8 tool positions on my turret (Hardinge CHNC) and I use them all. These are not individual tools like used with and Alaris tool holders.
I don't know enough about Mach to make my own screen sets, heck, I just figured out I can thread with my setup.
Thanks for the tips.
Vince
-
Vince,
Do you have any tool offsets in the tool table for tool#1 which is your master tool?
RICH
-
Vince,
I need to review my posted replies as they may need a few clarifications.
Later,
RICH
-
Also, I don't know what you mean by probing.
Vince
-
here:
https://www.youtube.com/watch?v=ewvp8jnof1E
is a good Video about probing.
-
What you really need to do is have a different reference. There is nothing sacrosanct about using Tool 1 as a reference, it's just convenient. My approach is to reference X to an accurate home switch that sets the machine zero at the start of every session; while Z I set with the tool I'm using to the end of the stock using a tool touch sensor. I do measure and store both X and Z offsets, but the latter are almost never used since I normally only use a single tool per program. So I can easily reset Tool1 offsets without affecting at least the X offsets for all the other tools. If you do want to use Tool 1 as the reference, then it's best to make it a "dummy" that's never used for turning - could be for example be made of mild steel just shaped for convenience in referencing.
Might also be useful to see this thread:
https://www.machsupport.com/forum/index.php?topic=39249.0 (https://www.machsupport.com/forum/index.php?topic=39249.0)
-
Vince,
If you watched the video you now know that probing is just a way of "automating the process" of how a tool
will touch a surface and provide data to the controller for using the different tools.
You can see that he modified the screen set to make it work for him. It is somewhat lacking in my opnion.
The best advice I can give to someone who is going to use a cnc lathe is study / educate themselves on the following:
- Tool geometry
- Different methods to touch off tools
- Tool offsets / tool table
- Work offsets
- Machine and Work offsets
Once the user is grounded in the basics much of the other stuff will fall in place. Time spent now will save you
hours later.
Later on the user can choose just what level of automation they require. Heck....I still don't use switches!
RICH
-
Thanks for the additional information. Is your probing routine part of Mach3 or an add on with a different screen set?
Vince
-
Vince, if you are asking me, it's a combination of a number of macros, some additions to the standard screen set (for example a button to "find stock end" on the manual screen), and a new offsets screen.
-
Vince,
I use a custom screen set which has numerous changes done to the Three Page Lathe Screen below.
Three Page Lathe Screen
https://www.machsupport.com/forum/index.php?topic=13548.0
I created a seperate Tool Setup page and on that page all tool probing is done. I use a simple tool setter
and probe to the appropriate surfaces. Additionaly I can probe to find lathe center, adjust probed offset
values, set a tool change location, but most importantly any lathe tool can be probed. By the way, a tool
setter does not need to be mounted in the chuck as it can be located anywhere as long as you can touch
off to it.
Additonaly that page allows for manipulation of the tool table such that it can opened/ saved / exported /
imported / reset / and recall a master tool table.
The screen set has two other pages which probe, one manualy and another automaticaly.
The manual one was done so I could do something quick and dirty to generate code, find points
along a profile ( whatever ) using a probe and create gcode or a dxf file. The other page is accuarte probing
to find points and generate a cad drawing based on the points. Very easy to duplicate a profile of something
with min amount of work. It beats scanning or the "bed of nails" approach!
Spent a lot of time, back a few years ago, reviewing anything having to do with probing and lathe screen sets
and just applied the best of the best to how and what "I" wanted.
RICH
-
Thanks for all the information. At this point with just my 8 tools, doing it manually is working fine. At worst if I change a tool I am looking at another 5 minutes to set it up. At some point I need to change out my computer (it's 20 years old). Which most likely means changing the BOB as well. I have an interesting set up with a PLC controlling the tool change carousel talking to the BOB. I put the system together 12 years ago and frankly don't remember exactly how it works. It would take a bit of study to change anything.
Vince