Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: mayhugh1 on November 03, 2013, 05:00:18 AM
-
I've been using MachTurn for several years but have just yesterday tried to make use of the tool tables. I've spent nearly 20 straight hours trying to make a run of 20 parts with three tools and am getting nowhere. Can someone point out what I'm doing wrong? Here is what I'm trying to do.
I set tool#1 in the tool window and I reference this tool to my part with skim cuts in x and z by setting the appropriate dro's on the manual screen. Then I put in tool#2 and I go to the offsets window where I set #2 in the tool number window and reference this tool to the same x and z surfaces. I press the 'touch' buttons which store the x and z offsets in the tool table. I look in the tool table and the offsets are there for t2 and zero for t1 as expected. I do the same thing for tool#3. I run the program and everything runs as expected. Then I put in a new workpiece and the problems start. I set tool#1 in the tool number dro on the manual page again and then I proceed to take skim cuts again on x and z and I reference the new surfaces in the dro's on the manual screen again. I realize doing the x again is likely redundant. Now when I restart the program, tool number one will not start cutting in the proper place in either x or z or both. I can try referencing tool#1 again and after several tries the tool may or may not start cutting in the proper place. I can't figure out what I'm doing wrong. It seems to only be t1 that has the problem. Once it is in the right place, the other tools are invariably correct. I've never had to re-reference t2 or t3. Can anyone tell me where I should be looking to fix this. Restarting Mach will let me re-reference t1 to the new workpiece but it seems I shouldn't need to do this every time is insert a new workpiece. - Terry
-
Hopefully one of the board gurus will be able to analyze your problem & straighten it out.
I had a terrible time with the tool table until I added a reliable and very accurate homing system and built a dial indicator center setting gauge for my lathe. I use the home position as zero and set my reference (tool #0) at zero. All other tools are set to an accurate spindle center point, & the offsets saved referenced to #0. As long as I remember to home the machine upon starting it up, it will hold .001" or better between all the tools. I do have to tweak the tool table a little to compensate for cutting different materials or changing insert types. My machine is pretty small & not as rigid as the "real" machines.
Here's a link to the center setting gauge. http://www.machsupport.com/forum/index.php/topic,25092.0.html
Milton
-
Have a look at Appendix "F" in the Lazyturn Manual which can be found in Members Docs.
I think you are creating an offset. Note that Milton uses a home position and i will remark that different folks
setup differently, but what is important is that you are consistant in what you do and it works for you.
Haven't used my cnc lathe for a couple of months now and hope to refresh my memory later today.
Remember that all tools are relative to a single tool but all the tools are also related to each other and Mach keeps track of the info.
I suggest you play a little, do exactly what you posted but every time you click a button or make a move just open the config >offsets
and see if something changed.
Later .......
RICH
-
I did a quick vid showing one method of setting tools up in Turn, might help.
http://www.youtube.com/watch?v=mWnfioI3G0E
Hood
-
Good vid Hood, way much better than trying to put it into words.
Don't care what they say about you, your allright....... :) :) :) :)
RICH
-
I found Hood's video while I was in the middle of trying to troubleshoot the problem and I seem to be doing everything that he is. My problem seems to be changing the master tool reference for some reason. Thanks, Terry
-
Don't care what they say about you, your allright....... :) :) :) :)
RICH
They can say what they like, and they DO!!!! and I dont give a Tom Tit :)
Hood
-
I found Hood's video while I was in the middle of trying to troubleshoot the problem and I seem to be doing everything that he is. My problem seems to be changing the master tool reference for some reason. Thanks, Terry
Please attach your xml and also your tools3.dat (it is in your profiles macro folder)
Hood
-
Hood,
Thanks for your help - I really appreciate it. Here are the files you asked for. - Terry
-
Here is the xml:
-
Can you also please attach your m6start and m6end macros please.
Hood
-
Hood,
Here is the m6start:
-
and the m6end
-
Dont see anything amiss in any of the files you attached so I think it must be your methodology that is the problem. I will have a read through your initial post again later on and see if I can understand where you are going wrong. I think it may be something to do with the way the lathe screen is, all these Home this and home that buttons.
I dont know what they are for to be honest as I used the standard screenset for 10 seconds and decided it was not for me so made my own.
Hood
-
Thanks for looking.
Let me repeat my process and maybe be a little clearer:
I type 1 into the T dro on the Manual screen. I insert my workpiece and take a skim cut on the end and then set the z dro to 0 on that same screen. I then take a skim cut on the diameter and then measure it and then set the x dro to that value on the same screen.
I then type 2 into the T dro on the manual screen and then touch tool 2 to the end of the workpiece. I enter the offset screen and type 0 into the z part-set dro and then hit the 'touch' button. This places the z offset into the tool table for tool 2 and I verify this by looking into the tool table. The offsets for T1 are both zero as I verify in the tool table also. I then go back to the manual screen where I can jog t2 to touch the diameter of the workpiece. I then go back to the offset screen and type the measured diameter into the x part-set dro. And then I hit the 'touch' button to set the t2 x offset in the tool table and I verify it.
I then repeat the above for tool 3.
I run my program and it runs to completion as expected.
I put in the new workpiece and re type 1 into the T dro on the manual screen. I jog the tool to touch the end of the workpiece and then I zero the z dro on the manual screen. I take a skim cut again on the new workpiece and enter the new diameter into the x dro on the manual screen.
I run the same program again and usually the tool t1 starts cutting at the wrong x or wrong z or both. I can re-reference the t1 in both x and y again a maybe that will correct the problem.
There is never a problem with running the program for the first time after a fresh reload of Mach. There is almost always a problem with running it a second time if a new workpiece is chucked and t1 referenced to it.
I never use the home buttons as I don't know what they do. And I seldom use the part set dro's on the manual screen as I usually just type directly into the dro's on that screen
Terry
-
I put in the new workpiece and re type 1 into the T dro on the manual screen. I jog the tool to touch the end of the workpiece and then I zero the z dro on the manual screen. I take a skim cut again on the new workpiece and enter the new diameter into the x dro on the manual screen.
You should not have to reset the X at all, unless of course you have restarted Mach and have no way of accurately homing.
Hood
-
Didn't get around to foolling with the lathe yesterday but will today and will follow what you did in reply 14.
So from memory let me say a few things and make an ask out of my self...............
Clicking the Zero World X and Z buttons will remove any WORK offsets that were created or saved and resets the DRO's to zero.
So if you now move the axis the DRO's will change reflecting the movement. So wherever the tool is located within the travel limits
of the axis ( by tool I am refering to the controlled point which is the point of the tool which actualy cuts the material), x&z=0 is based on where you were at the time you clicked the Zero World buttons. If you move away from 0,0, stop somewhere,
click the Set Home X & Z buttons, you have just told Mach that this is a location away from 0,0 which is home relative to 0,0 and within the travel limits.
So we now have Z & X =0 defined, and also have a home location defined within the travel limits.
If you move the axis away from home, stop, and then click the Home All button, the axes will move back to where you set home.
G28 in the MDI ( do some reading on how G28 is used). You can use the Home x or z buttons for the individual axis to go back to home.
------------------------------------------
So you have a bunch of tools which were setup based on a master tool, say T1, they a numbered on the tool holder so you can't mix them up . All the other tools are based on T1.That master tool is never used for cutting, thus no wear / the controlled point never changes. You use the master tool to setup the lathe.
So all you need to do is read section 4.5 of Appendix "F" in the Lazyturn Manual which can be found in Members Docs. You simply create a work offset
(IE;G54) THUS THE TOOL TABLE IS IS NOT AFECTED.
Hope I didn't confuse,
RICH
-
Hood,
I've gotten into the habit of re- referencing both axes because my lathe isn't all that rigid and I've found that during a long cutting program the x reference can wonder around several tenths and if I reset the x with each new workpiece I can keep the accuracy a little better under control. Also due to deflection, if I don't run my skim cut at the same doc as my final finish cut on the part, I won't be accurate on the final finish diameter. When I tried to reference my x for my second and third tools, I jogged step at a time up to the workpiece diameter until (by rotating the spindle by hand) I start to rub off the machinists dye on the diameter of the skimmed part with the tool to be referenced. Maybe my workflow isn't what Mach is expecting and I'm running into some subtle problem with the software. Rich - I have to study your reply more carefully. There's more in there that I have to think about even though I have read that appendix several times already.
Thanks all, - Terry
-
A few thoughts Terry,
Once you set the tool table up the first time you should not do anything that is changing the differences between them. Of course if you
break or dull the tool you need to change the tool table by going thru the sequence of touching off the tools, or if you have a tool setter then change the particular tool offset manualy. Depends how you work , but if you use a work offset, you won't see a difference in the tool table because you didn't do anything to screw it up. The only difference is the location of the master tool from the part.
Also if you keep the values of the tool table after they are touched off you could always just change the tool table manualy, apply / save, if you do something that screws it up.
An exercise worth doing is to create the tool table, then check to see if there are any work offsets, then do what you want, but ONLY ONE STEP / or CHANGE at a time and see what the affect was ie; did the tool table values change, did the dro values for program/part/machine change, is there a fixture offset / is it different, what happens if one just changes the tool number while at home or at soem location, etc. You will learn a lot and it will keep out of the bars! Ou also should take a look at the first move depending on how the code was created ie; wizard
use and using diameter or radius mode and current Mach settings.
Frankly, it can get confusing quick especialy if you need to change screens to do things ( i use a modified lathe screen).
Remember all this is a fun thing, ;)
RICH
-
Another interesting thing is how (or if) G49 works in MachTurn. I don't believe it does anything. For example, I can reference my tool1 and go ahead and set the offsets for tool2. If I then switch to tool2 (enter T2 in the tool dro) I can see the dros change to reflect the offsets for T2 compared with T1. If I MDI G49 nothing happens on the T2 dros. In the mill software, the dros change to reflect the cancellation of the length offsets. In Turn there is no apparent effect. It seems the only way to cancel the length offsets is to MDI T0101 or MDI T0000 or to enter T0 or T1 into the tool dros. I see many Turn programs that start out or end with a G49 in the machine setup block, but does it really do anything? - Terry
-
Tool offsets in Turn are different from Mill, they are controlled via the last two digits in the tool call, so for example T0101, T0801, T9901 would all bring up the same values into the X and Y DRO, ie the offsets of entry 1 in the tool table.
Hood
-
Hood,
So are you saying that you too don't think g49 does anything in Turn?
Thanks,
Terry
-
I have never tried it but I dont think it does as there is not really a Length Offset in Turn, the offsets are X and Z and are applied by calling the tool offset from the tool table, so the way to cancel is call a 00 for the last two digits of a tool. That could be by calling the same tool as you currently have in but with 00 as the ofset portion or by possibly calling T0000. The latter however likely wouldnt work if you have an auto changer (turret/tool post) as most likely that would be out of range.
Hood
-
It's interesting because one of the options in the General configuration panel in the Turn profile is to opt for a G49 and/or a G40 when the end of a program is encountered. At first I thought this might be related to my problem and what you were looking for in my profile, but it didn't seem to help. - Terry
-
The thing is, originally Turn was just Mill with a few tweaks. For example you used to call a tool and offset in the same manner as you do in Mill. It was changed long ago to adopt the normal convention for Lathes and likely these options are just artefacts from the original method. For example to tool table still has 250 odd offsets, you can only use 99 of them for lathe however.
Hood
-
Hey Hood,
While watching your video I liked your touch off indicator. So having an extra center finder for the mill decided to try
it out for the lathe. The tape just keeps end of the finder centered and restricts movement. The accuracy for setting lathe tools was exceptional, and although I have a microscope on the carriage, touching off to the center finder is so much quicker.
Pic attached......
RICH
-
Looks good Rich, I was considering using an edge finder at the start but the only one I had was the sprung ball type, so not much use. As I am Scottish I got a fever when thinking about the cost of purchasing a new cylinder type one for this so I decided to make my own ;D
Actually the real reason I made one is the Hyd chuck likely would have crushed the edge finders body through time.
Hood
-
Hey Hood,
While watching your video I liked your touch off indicator. So having an extra center finder for the mill decided to try
it out for the lathe. The tape just keeps end of the finder centered and restricts movement. The accuracy for setting lathe tools was exceptional, and although I have a microscope on the carriage, touching off to the center finder is so much quicker.
Pic attached......
RICH
I always thought this would be the best way to set up tools. Just seems easy.
Btw the tool table and offsets configuration is difficult to say the least. I can remember a phone call from a member here who used the analogy, if Lupe was on the 50 yard line. The story never made sense but somehow I did learn to load my tool table to some degree, practice would of course would make me better at it.
I did pick up one tidbit on this thread, to use a non tool as the reference/master. I had read this before but ignored it and used my longest tool as the reference. All of a sudden during reading this thread it dawned on me (just before reading Rich's remark about non tool for the master) what happens if I broke tool 1 or it had significant wear? Slow learner? Damn I hate that. I guess learning it at some time is better than never.
-
I'll post some info in Member's Doc's on setting up the tool table.
Found the file I posted for Fastest1 some time ago, thought I put in Members Doc's, but it never got there.
I think I understand what the difficulty about the tool table is and will try to address it.
Later,
RICH
-
IIRC my biggest problem was pressing some button on the offsets or tool table page that only was to be pressed for setting up the Master Tool every tool after that had a similar process but didn't need that button pressed.
Just going back thru the pages I don't see the obvious button, only 1 is to be used to set the master.
Rich we might be talking about Lupe soon ;-)
-
Fastest,
Consider the following:
1. Different lathe screens
2. Different ways of holding the tools ( ie; turret, quick change, multiple tool holding bar)
3. Different machine setups ( ie; no home switches, home switches, using soft limits, etc)
4. Different techniques to touch off the tool
5. Lots of buttons on the screen ( who reads a manual to learn what they are for or what happens when you tick one )
6. Who reads the manual to understand the logic of the different coordinate systems, offsets, configuration, etc.
The list can go on and on, but, as far as the tool table is concerned, they all have a BASIC thing in common,
namely........ each tool has an X and Z offset from a reference.
So, if you forget about all the considerations listed above, focus on just the tool / populating the table and grasp the basic concept, the tool table itself becomes rather simple. ???
LATHE TOOL TABLE BASIC CONCEPT
The tool table is just a listing of the distances the tools are from some location. The same location is used for all the tools.
One tool is used to define the location to the software and then all the other tools are moved to that same location to
find the difference in distance they are from that location. Each tool distance is stored in the tool table for use by the software.
RICH
-
There are a number of ways to populate the tool table.
1. Use a tool settting fixture ( Don't think most folks have one ) which will provide the required info to populate the tool table
manualy.
2. Use Mach to find the distance differences each tool is away from a reference point, record the info and enter the info manualy
into the tool table.
2a. Same as 2, but, tick a few buttons to transfer info to the tool table.
Before a user even tries to get the tool table populated they need to do a few things.
1. Label each tool and make sure the tool is set at the proper heigth.
2. Set up a few software configurations
3. You will need a reference to touch off the tools or you can machine something to be used as a reference.
RICH