Hi folks, I have some question, so I am using Mach3 Turn in radius mode to control Emco Turn 220 P lathe with rear turret tool changer, also I bought Partmaster Lathe V13 from Dolphin USA, I had troubles to get post processor that supports peck drilling (something was wrong in existing post processors), anyway got post processor that supports peck drilling and few days I ago when I manage to make some tools that I can fit in turret (small lathe ,even smaller tools) I went to cut some test parts. So first thing is that I learned how to offsets tools (I measured values and entered them in Mach3 Tool Table and in CAM also where you make definition of your tool, seams very intuitive, I mean how will CAM know how much drill in turret should be backed off if you do not enter offset ). So to me was logical that what I see in CAM will correspond in reality. In CAM setup you can define safe place for tool cahnge operation, I chose z=8, x=30 according to inserted work piece and mounted tools in turret (1 profiling tool (master tool), center drill, drill 7.2 mm and parting off blade). So after some testing I realized that only master tool correspond to what I can see in CAM when I give command for tool change, rest of 3 tools (total tools can be eight) are "randomly" positioned in space, I do not know better word then randomly (there is some logic but I can not follow it so will use word randomly), thing is that for example I see tip of drill in CAM positioned in places (z=8, x=30 , safe place) and in reality it is somewhere out of that place so I can not plan movements where I want each tool to go, what to machine. Also in reality for given profile , machine with those 4 tools part will  machine parts but it is question will I brake some tools or will I damage spindle and chuck because paths that I see in reality can not be seen in CAM.

I also made video where I showed what is happening and described what I am trying to ask, what should I change, should I change or ask Dolphin USA to make changes , anyway in which direction need to go.

My experience with Gcode is almost zero, I manage to make macro for operating tool changer , basically, I jog tool changer some where in working area and I type T0101 , T0202... to T0808 and turret only rotates and I got chosen tool. I thought maybe I need to make in macro some movements but that did not seems logical to me me because , in CAM already exist places where you need to enter x an z offests and it is easier to use and update that information then to adjust macro every time when you machine different part.

Also I entered tool offsets to be same in Mach3 Tool Table  and in CAM because I read on forums that it should be done like that , and when I run out of ideas I tried to delete offests of all tools in CAM , I thought maybe it will work (what I see in reality will be in CAM) but nothing has changed, you can see that in video.

So first video is connected with my question and second video is rewind  so yo can see what happens in reality when you see in CAM one thing and in reality something else.

https://www.youtube.com/watch?v=oqk1cWgOqq0

https://youtu.be/0JFMlsJi12I

I got this from support:

"This is really a MACH3 issue, but there are some things to bear in mind.
 
In PartMaster – don’t enter any values into the Tool Offset boxes...... they will be ignored.
They are only there for very, very old controllers that don’t have tool offset capabilities.
 
image
 
All tools offsets MUST be set on the machine – MACH has a tool table that allows you to enter the offsets to be used when the tool is selected.
 
The MACH3 forum is the best place to get this orted."

And my replay to support:

"Hi , thx for replying back. I start to study all about editing post processor for Partmaster Lathe and I noticed that in post processor that I got for Mach3 Turn there does not exist key word TURRET and in old post processor (I will attach both ) there exist key word TURRET but post processor did not performed peck drilling and deep drilling operation. I was thinking what I would love or I think that machine would need to do, for example when I choose change from profiling tool to drill, I think that turret (tool changer should) back off for length of tool in Z positive direction and after that it should rotate to chosen tool, in that way machining would match what I see CAM, for parting tool, tool should retract in x positive direction before changing to next desired tool. I do not want that those things are happening all the time, I just want them when  is generating g code in CAM for auto mode in Mach3 Turn, I should make changes in macro but then every time when I would give command for tool selection (when I am in manual mode), turret would be moving up or right depending on current tool type, so because of that my conclusion is that probably those thing should be adjusted/built in post processor because in CAM I chose safe tool changing position and according to that position turret back off up or right for tool offset value. I hope you can follow what I am talking about, are there any commands with  which I can in post processor set back off in x or z direction and is there any command that give me information of type of tool that is chosen for each CAM operation (I want to get information current tool is drill and in that case I need to move back first in z positive direction first and after in x direction depending of value off offset to comparing to master tool).

Wise tool offsets, I entered them in Mach Tool Table and both in CAM in tool definition because I read on forum that it should be done like that but when I saw that machine does not acts like in CAM 2 d simulation I went to test what will happen when is set offset to zero , what now agrees whit what you are saying.

So I was looking in those 2 post processor and they look quite different to me, I needed one for Mach3 Turn in radius mode, and I got probably generic one for Fanuc controller, it say in description it is for colechsther late with one rear turret. So is it possible to make that logic in post processor for CAM, I mean I first need to know does exist commands that can give me information of type of tools and how much is value of offset for given tool so I can make some logic where to move first.

Till now no replay on CNC zone and Mach support forum."

Whatever CAM package you use does not need to know about tool offsets. Dolphin support is accurate in their comment that tool offsets are only needed for old controllers that do no support tool offsets.

As far as the CAM is concerned, it requests a tool, and the machine controller (Mach in this case) handles all the offsets.
For example, if you want to turn something 10mm diameter with tool 2, the CAM will produce some code to tell Mach to change to tool 2, then move to X10 (in diameter mode).
If your post processor is also applying tool offsets, then that is most likely why you are getting 'random' positions.

If you can show us an example gcode file (either attach it, or copy and paste), it will give us a far better idea of what is happening.

Whatever CAM package you use does not need to know about tool offsets. Dolphin support is accurate in their comment that tool offsets are only needed for old controllers that do no support tool offsets.

OK, for that , it is even better , I do not need to enter 2 time same data, and like said and showed in video above, I confirmed that by myself even I did notknow that fact, I thought something is wrong.

As far as the CAM is concerned, it requests a tool, and the machine controller (Mach in this case) handles all the offsets.
For example, if you want to turn something 10mm diameter with tool 2, the CAM will produce some code to tell Mach to change to tool 2, then move to X10 (in diameter mode).
If your post processor is also applying tool offsets, then that is most likely why you are getting 'random' positions.

If you can show us an example gcode file (either attach it, or copy and paste), it will give us a far better idea of what is happening.

Another fact is I would get machined profile , and drilled holes in reality like it is in CAM, only problem is that paths in reality are different then what is see in CAM, and reason is that tools rotate in turret and in CAM that fact is not considers, is not took in calculation, I can use GOTO button in CAM to avoid collisions with spindle or part in chuck but it is frustrating because you do not know will you hit soft limits or you will not raise tool changer high enough in order to avoid crashing drill in spindle and so on.

It would be nice when CAM would take care of those things, and I think why not, if it have access of tool offsets and type of tools, you need to define each tool that you will be using, how wide it is, long, etc. I will try to explain in different way by pictures, I know it is not easy to understand when you do not have machine in front of self and part in CAM so you can run simulation and code.















By random positions I meant deviation from what I see in CAM, I mean how can you plan something, where to tool goes when starting point of tool in reality is offset

to some other place different then shown in CAM, and it did not took double offsets, it does not makes difference do I enter tool offsets in CAM or not in tool definition setup widows.

I hope it is more clear now, I did not make pictures for complete G code because parting tool is not so dangerous as drill bit

Sorry for large pictures  

and G code

;(klizac7mm.cnc)
N20G21 G18 G64 G80 G90 M49 G90.1 G40 G49
; TOOL definition
N40 M09
N50 G00 X30.0 Z8.0 M05
N60 G49
N70 ( Turning tool )
N80 T0101
N90 M03 G94 F500.0
N100 G97 S1500
N110 G00 X6.649 Z0.306
N120 G01 Z0.108
N130 X0.893
N140 G00 X3.712 Z1.134
N150 X6.649
N160 Z0.306
; TOOL definition
N180 G00 X30.0 Z8.0 M05
N190 G49
N200 ( Centre Drill  10mm Dia )
N210 T0404
N220 M03
N230 S1500
N240 X0.0 Z3.0
N250 G01 Z-2.0 F200.0
N260 G00 Z3.0
; TOOL definition
N280 G00 X30.0 Z8.0 M05
N290 G49
N300 ( Twist Drill / Center Drill  7.2mm Dia )
N310 T0606
N320 M03
N330 S1500
N340 X0.0 Z3.0
N350 G01 Z-22.4
N360 G00 Z3.0
; TOOL definition
N380 G00 X30.0 Z8.0 M05
N390 G49
N400 ( Turning tool )
N410 T0101
N420 M03
N430 S1500
N440 X3.334 Z3.038
N450 G01 X2.535 Z2.087
N460 G02 X3.596 Z0.05 R1.243
N470 G03 X3.625 Z0.043 R0.05
N480 X6.05 Z-3.927 R4.854
N490 Z-3.93 R0.05
N500 G01 Z-4.242
N510 G03 X5.816 Z-4.693 R0.55
N520 G01 X4.843 Z-5.374
N530 G02 X4.75 Z-5.669 R1.084
N540 G01 Z-13.066
N550 G02 X5.642 Z-13.87 R1.318
N560 G03 X6.05 Z-14.402 R0.55
N570 G01 Z-14.748
N580 G03 Z-14.752 R0.05
N590 G01 X5.825 Z-18.002
N600 Z-24.0
N610 G03 X5.804 Z-24.041 R0.05
N620 G02 X6.301 Z-26.283 R1.243
N630 G01 X7.524 Z-26.498
; TOOL definition
N650 G00 X30.0 Z8.0 M05
N660 G49
N670 ( Grooving tool / Partoff blade )
N680 T0707
N690 M03
N700 S1500
N710 G00 Z-26.671
N720 X6.387
N730 G01 X-0.149
N740 G00 X6.387
N750 M05
N760 M30

Whatever CAM package you use does not need to know about tool offsets. Dolphin support is accurate in their comment that tool offsets are only needed for old controllers that do no support tool offsets.

OK, for that , it is even better , I do not need to enter 2 time same data, and like said and showed in video above, I confirmed that by myself even I did notknow that fact, I thought something is wrong.

As far as the CAM is concerned, it requests a tool, and the machine controller (Mach in this case) handles all the offsets.
For example, if you want to turn something 10mm diameter with tool 2, the CAM will produce some code to tell Mach to change to tool 2, then move to X10 (in diameter mode).
If your post processor is also applying tool offsets, then that is most likely why you are getting 'random' positions.

If you can show us an example gcode file (either attach it, or copy and paste), it will give us a far better idea of what is happening.

Another fact is I would get machined profile , and drilled holes in reality like it is in CAM, only problem is that paths in reality are different then what is see in CAM, and reason is that tools rotate in turret and in CAM that fact is not considers, is not took in calculation, I can use GOTO button in CAM to avoid collisions with spindle or part in chuck but it is frustrating because you do not know will you hit soft limits or you will not raise tool changer high enough in order to avoid crashing drill in spindle and so on.

It would be nice when CAM would take care of those things, and I think why not, if it have access of tool offsets and type of tools, you need to define each tool that you will be using, how wide it is, long, etc. I will try to explain in different way by pictures, I know it is not easy to understand when you do not have machine in front of self and part in CAM so you can run simulation and code.



By random positions I meant deviation from what I see in CAM, I mean how can you plan something, where to tool goes when starting point of tool in reality is offset

to some other place different then shown in CAM, and it did not took double offsets, it does not makes difference do I enter tool offsets in CAM or not in tool definition setup widows.

I hope it is more clear now, I did not make pictures for complete G code because parting tool is not so dangerous as drill bit

I resized pictures and I forgot to insert chunk in one picture.















and G code

;(klizac7mm.cnc)
N20G21 G18 G64 G80 G90 M49 G90.1 G40 G49
; TOOL definition
N40 M09
N50 G00 X30.0 Z8.0 M05
N60 G49
N70 ( Turning tool )
N80 T0101
N90 M03 G94 F500.0
N100 G97 S1500
N110 G00 X6.649 Z0.306
N120 G01 Z0.108
N130 X0.893
N140 G00 X3.712 Z1.134
N150 X6.649
N160 Z0.306
; TOOL definition
N180 G00 X30.0 Z8.0 M05
N190 G49
N200 ( Centre Drill  10mm Dia )
N210 T0404
N220 M03
N230 S1500
N240 X0.0 Z3.0
N250 G01 Z-2.0 F200.0
N260 G00 Z3.0
; TOOL definition
N280 G00 X30.0 Z8.0 M05
N290 G49
N300 ( Twist Drill / Center Drill  7.2mm Dia )
N310 T0606
N320 M03
N330 S1500
N340 X0.0 Z3.0
N350 G01 Z-22.4
N360 G00 Z3.0
; TOOL definition
N380 G00 X30.0 Z8.0 M05
N390 G49
N400 ( Turning tool )
N410 T0101
N420 M03
N430 S1500
N440 X3.334 Z3.038
N450 G01 X2.535 Z2.087
N460 G02 X3.596 Z0.05 R1.243
N470 G03 X3.625 Z0.043 R0.05
N480 X6.05 Z-3.927 R4.854
N490 Z-3.93 R0.05
N500 G01 Z-4.242
N510 G03 X5.816 Z-4.693 R0.55
N520 G01 X4.843 Z-5.374
N530 G02 X4.75 Z-5.669 R1.084
N540 G01 Z-13.066
N550 G02 X5.642 Z-13.87 R1.318
N560 G03 X6.05 Z-14.402 R0.55
N570 G01 Z-14.748
N580 G03 Z-14.752 R0.05
N590 G01 X5.825 Z-18.002
N600 Z-24.0
N610 G03 X5.804 Z-24.041 R0.05
N620 G02 X6.301 Z-26.283 R1.243
N630 G01 X7.524 Z-26.498
; TOOL definition
N650 G00 X30.0 Z8.0 M05
N660 G49
N670 ( Grooving tool / Partoff blade )
N680 T0707
N690 M03
N700 S1500
N710 G00 Z-26.671
N720 X6.387
N730 G01 X-0.149
N740 G00 X6.387
N750 M05
N760 M30

The CAM is doing exactly what you're telling it.
You've set it to move to X30 Z8 for the currently selected tool, prior to carrying out a tool change, which means the next tool position will be relative to the previous tools position.

What you really want, is for the turret to move to a safe position using machine coordinates, so the next tool position is not dependant on the last tool position.
This is normally done by adding a G53 to the G0 move prior to a tool change, for example -
G0 G53 X0 Z0 (move to machine home)
T0101 (change to tool 1 with tool 1 offsets)

There will be an option somewhere within Partsmaster to configure what offsets/codes get used for a tool change, however I personally don't know.

The CAM is doing exactly what you're telling it.
You've set it to move to X30 Z8 for the currently selected tool, prior to carrying out a tool change, which means the next tool position will be relative to the previous tools position.

What you really want, is for the turret to move to a safe position using machine coordinates, so the next tool position is not dependant on the last tool position.
This is normally done by adding a G53 to the G0 move prior to a tool change, for example -

Code: [Select]

G0 G53 X0 Z0 (move to machine home)
T0101 (change to tool 1 with tool 1 offsets)

There will be an option somewhere within Partsmaster to configure what offsets/codes get used for a tool change, however I personally don't know.

Hi, thx for replay again, will try to explain how I feel things. So you/I/we  want to make part like for example shown on pictures above, you know which tools you need and you need to measure them (for drill how much it sticks out of turret, which diameter it is, and off course you need to enter tool offsets in Mach3 Tool table. Next step is to take in count how much sticks part that you machine out of chuck, how big is your chuck and how much is longest tool in turret and how much maximum stick out of torturer some particular tool. And when you take all those things in a count you go in CAM in setup machine (you open tab) and you define Safe home position (and CAM need to do some things not only G00 X30.0 Z8.0 M05, at least I think so) , which is in my example, x=30 and z=8, so according to that point I see in CAM in graphic interface paths for every single operation(it is not easy to follow paths if you have lot of operations), and every operation starts from that point, and I want to adjust post processor (In worst case I will need every time in Mach3 macro make changes to get what I want , and to me it is not smart way to go, maybe it is easiest) to in reality get that for every new machining operation tool tip start in (x =30, z =8) which is safe and optimal point.

So :

"The CAM is doing exactly what you're telling it."

Is relatively true, machine (tool changer) goes to place what controller reads in  Gcode, but thing it that I do not want that CAM(post processor)  simple write :

N280 G00 X30.0 Z8.0 M05
N290 G49
N300 ( Twist Drill / Center Drill  7.2mm Dia )
N310 T0606

I want to adjust post processor in this way, OK currently active tool is center drill, next will be in use tool N0 7, it is type of tool drill (everything is defined in CAM setup, how long it is and diameter....) according to this type of tool extract somehow tool offsets for that tool,then I need (post processor needs)to retract complete tool changer first in plus absolute z tool offset value for tool N0 7 in direction and after that in positive or negative x direction and after those two retraction I can execute rotation of turret and tool tip will be precisely in coordinates
(x =30 , z = 2)

G0 G53 X0 Z0 (move to machine home), thing with this (I did not tried) but I think that if I will use that machine would want to go every time in some fix point in space that will be safe but there is no need to go every time to that place because some tools do not stick so much that I need to go on place to avoid worst case scenario tool.

Like I said I am newbie with Gcode so maybe I do not understand possibilities well . I would love to hear is this possible to make that what I have in my head because when I play in CAM everything tells me it should be like that.

So machine fallows exactly what is in Gocde but thing is I want to post processor generate different G code.

Before you worry about doing multiple parts, learn the basics.

I only used G0 G53 X0 Z0 as an example, you can change tool anywhere.
A major benefit of not having a fixed tool change position (i.e. coding it into the M6 macro), is you can command a tool change anywhere, however it is then up to you to ensure any tool changes are done in a 'safe' position. Some CAM packages are capable of doing that, however it normally means the CAM package has access to a 3D model of the machine, so it can simulate changes and know how much clearance is needed. But such CAM packages are expensive, and even more time consuming to setup.

Normally you'd pick a point where everything is clear of the spindle/work piece for all tools, however if you're wanting to minimise cycle time as much as possible, you can take the generated g-code from the CAM, and manually alter the tool change positions. However you would only normally do that if you're expecting to run a high quantity of identical parts, as it could easily take you 10-15minutes to find the optimum tool change positions, yet only save seconds of each cycle time, and you also risk the possibility of getting it wrong and causing a crash.

Regarding doing multiple parts, you can either rely on the CAM to simply generate additional lines to machine additional parts nearer the chuck, or re-use the code but insert temporary/work offsets to move everything nearer the chuck. However, before you get to that level of complication, learn and understand how to make single parts first.

Another option is to modify your M6 macro, so a move occurs to move the tool to the same X and Z tool position as the previous tool. I.e. if the last tool was at X30 Z8, the M6 macro would move so the new tool is at X30 Z8, prior to completing the tool change.
However, you run the risk of hitting a limit, if the difference between offsets exceeds machine travel.

Another option is to modify your M6 macro, so a move occurs to move the tool to the same X and Z tool position as the previous tool. I.e. if the last tool was at X30 Z8, the M6 macro would move so the new tool is at X30 Z8, prior to completing the tool change.
However, you run the risk of hitting a limit, if the difference between offsets exceeds machine travel.

Yes you are right, I agree with that 100% , this is why I wrote in  worst case I will need to enter Mach3 macro, plus I want to tool changer when I am in manual mode acts like it acts now, to only rotate turret, I do not want that for every tool change command is on different position, in that way would be pain in ass to determine safe place for tool change in CAM, so that is last thing I want to try. Hope on forum is some one who know something about Partmasters post processor. I really appreciate your replay, even you do not know how to adjust post processor .