Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: BGelektronika on January 09, 2020, 10:41:16 AM
-
Hello,
I have problem how to setup tool change, as tool charger is here located in Y axis. I have modified screen and added Y axis, so with JOG or with MDI command all axis are working and showing in program also homing...
So the question now is how to save diferent tools and than call it from MDI?
I really kindly asking for help.
Thank you
Best regards
Gasper
-
You have a modified screen set so not sure what happens when you click one of the buttons.
Generally, use the Master Tool concept and populate the tool table.
Once the tool table is populated you can call the tool you want to use.
Have a read of good read ( study would be a better word than read) "Using Mach3 Turn" manual since it covers most of all the basics that you will need to know.
RICH
-
Dear Rick, Thank you for answer.
However, Mach3 Turn manuals doesn't help much as turns usually don't have Y axis.
I have try to change screen like in this topics:
http://www.machsupport.com/forum/index.php?topic=35814.0
but then I have found this topics, and here is also Yaxis lathe.
http://www.machsupport.com/forum/index.php?topic=21851.0
So Can and If yes, how to use this M6 macro to work with my machine.
Thank you
Best regrads
Gasper
-
but then I have found this topics, and here is also Yaxis lathe.
http://www.machsupport.com/forum/index.php?topic=21851.0
So Can and If yes, how to use this M6 macro to work with my machine.
i think this macro's are a good base to start with.
you will have to design a custom screenpage where you can set your y-axis values.
X and Z Offsets will be covered by Standard tooltable.
in this example M6Start macro toolpositions are stored in OEMDRo's
toolpos1 = GetOemdro(1001)
toolpos2 = GetOemdro(1002)
...
...
and the it drives the y-axis to the defined value for each tool in machine coords
If (toolnew = 1)then
Call Code("G0 G53 X105 Y4.5"&(toolpos1))
While ismoving()
Sleep 100
Wend
End If
it also moves the X and Z axis to a tool Change position
Call Code("G0 G53 X105 Y4.5"&(toolpos1))
i personaly would do this in two step's, first move X and Z out the collision aeria and then move Y,
or maybe in three step's 1.X 2.Z 3.Y or 1.Z 2.X 3.Y to make sure the is no collision possible.
-
I am putting some info together for you that will answer your how to question.
RICH
-
Thank you all for answers.
If I use that M6 macro what else I have to do to get it work, coz nothing happens if I write T01 ..... in MDI, or I get invalid tool number message.
Do I need to add something on screen? I'm completely lost now...
So any help is really useful, coz without that machine is useless.
Machine is on CsLab CSMIO IP controllers if that change anything.
Thank you
Best regards
Gasper
-
Looking at your tool holder looks like you have the ability to have 10 tools in the holder.
You will need to have a custom M6Start macro. The M6 macro provides scripting / code to do whatever you want to do. So as TPS points out, you need to think about how YOU want a tool change to work.
Need to decide on whether the lathe will be a front or rear tool post since you should not, do not, never, mix front or rear tool post definitoin in the tool table. Choose one or the other not both.
So think about the above and i'll post info that you need to know and be aware of about tools and
configuration, etc.
RICH
-
in turn mode code for toolchange is:
M6 Txxyy where xx is the tool # and yy is the offset .
-
Yes it have 10 tool holders.
It will be always used as rear post.
-
Attached PDF is basic info / generic for the lathe.
With a custom screen set like yours I would suggest that later on you consider adding a page where you can do tool set up. In that screen create the ability to probe your tools to populate, manipulate, change the tool.
It is fast, very accurate, etc.
RICH
-
It will be always used as rear post.
If I recall the rear tool post uses G55 Work offsets for the tools offsets.
So be carefull with your work offsets.
RICH
-
Remember also that the Lathe tool table is in terms of radii. Machine Coordinates are in radii.
You need to define what lathe mode you want use.
FWIW,
RICH
-
I manage to get macro work, so I can chose all tools now. But when a chose any toll lat say T0202, machine only move for X,Y,Z written in M6 macro, it doesn't move for offsets I put in tool table. In screen I see requested tool and offset are shown in DRO for requested tool, but machine don't move for offsets.
-
the X,Z Offset will be captured by the next move after toolchange, the toolchange itselve will only "correct" the DRO's/coordinates (for this axis).
-
but then I have found this topics, and here is also Yaxis lathe.
http://www.machsupport.com/forum/index.php?topic=21851.0
So Can and If yes, how to use this M6 macro to work with my machine.
i think this macro's are a good base to start with.
you will have to design a custom screenpage where you can set your y-axis values.
X and Z Offsets will be covered by Standard tooltable.
in this example M6Start macro toolpositions are stored in OEMDRo's
toolpos1 = GetOemdro(1001)
toolpos2 = GetOemdro(1002)
...
...
and the it drives the y-axis to the defined value for each tool in machine coords
If (toolnew = 1)then
Call Code("G0 G53 X105 Y4.5"&(toolpos1))
While ismoving()
Sleep 100
Wend
End If
it also moves the X and Z axis to a tool Change position
Call Code("G0 G53 X105 Y4.5"&(toolpos1))
i personaly would do this in two step's, first move X and Z out the collision aeria and then move Y,
or maybe in three step's 1.X 2.Z 3.Y or 1.Z 2.X 3.Y to make sure the is no collision possible.
I would really like to make script in 3 steps 1.X 2.Z 3.Y.
I kindly ask you if you could make quick look how should script look like, only for one tool, I will than modify myself for other tools.
I need to get modified this part:
If (toolnew = 1)then
Call Code("G0 G53 X105 Y4.5"&(toolpos1))
While ismoving()
Sleep 100
Wend
End If
Thank you
-
If (toolnew = 1)then
Code "G0 G53 X105" 'move X-axis
While ismoving()
Sleep 100
Wend
Code "G0 G53 Y"&toolpos1 'move Y-axis
While ismoving()
Sleep 100
Wend
Code "G0 G53 Z105" 'move Z-axis
While ismoving()
Sleep 100
Wend
End If
you have to replace the 105 with your machine coords you whant to use!!!!!!!!!
-
If (toolnew = 1)then
Code "G0 G53 X105" 'move X-axis
While ismoving()
Sleep 100
Wend
Code "G0 G53 Y"&toolpos1 'move Y-axis
While ismoving()
Sleep 100
Wend
Code "G0 G53 Z105" 'move Z-axis
While ismoving()
Sleep 100
Wend
End If
you have to replace the 105 with your machine coords you whant to use!!!!!!!!!
Great thank you so much
-
Can someone please explain me what is mean "&toolpos1 coz I have problems with Y height. Sometimes it goes to much up, and for tool 3 it goes all the way to the limit switch. If I delete &toolpos1 for all tools in m6start macro, then are all on the right position. So where is the catch?
Thank you
-
toolpos1 to toolposx are coming from OEMDro's at beginning of code
toolpos1 = GetOemdro(1001)
toolpos2 = GetOemdro(1002)
...
...
so you have to create a custom Screen, where you can set the Dro's corresponding to your particular tool.
this line of code
Code "G0 G53 Y" & toolpos1 'move Y-axis
is only the combination of fix code, in this case "G0 G53 Y" added by the "&" and value of variable toolpos1
let's value of toolpos1 = 1234 the excecuted code would be
G0 G53 Y1234
maybe you can post your actual code.
-
Thanks to you guys, i have manage to setup tool change perfectly.
I would just like to make minor change in m6start macro, but I'm not sure if its possible.
This is tool1 :
If (toolnew = 1)Then
Code "G0 G53 X38" 'move X-axis
While ismoving()
Sleep 100
Wend
Code "G0 G53 Z-113" 'move Z-axis
While ismoving()
Sleep 100
Wend
Code ("G0 G53 Y66."&(toolpos1)) 'move Y-axis
While ismoving()
Sleep 100
Wend
End If
So I have fixed Y at 66 and then i get 0.*********xx from 1001 dro from my screen. So I can make minor adjustment on screen dro.
The question is, is it possible that my 1001 dro number change Y for +or- number intered in1001 dro? SO let say I have fixed Y66 from M6 macro, and I enter 10 in 1001 DRO, and that change actual position from Y66 to Y76.
Thank you
Gasper
-
if you use
Code "G0 G53 Y"&toolpos1 'move Y-axis
insted of your code and you can enter numbers directly to dro 66.123 will be 66.123 in real
if you want an Offset to 66 use
temp = 66 + toolpos1
Code "G0 G53 Y"&temp 'move Y-axis