TurnMill

[D&S PRECISION]

hi folks....

 

i try to making round pocket on od offsetting in Y+ direction in the new turnmill machine with Y. i am using mastercam 9 and x5. i dont want to use the cross contour in the c axis toolpaths. what i want to do though is to ramp-in to full depth and machine the entire pocket. Any help will be appreciated......

[Josh Kinney -Elite Engineering]

I honestly never use the c-axis toolpaths. Just use a mill toolpath.

[CJep]

If you have a post, machine & control def loaded capable of 4axis lathe functions, such as the mplmaster, generic 4x mplfan,...

You may notice that in the lathe toolpath drop down of McamX5 that there is access to the "mill" toolpaths just below the "c-axis" toolpaths.

 

If you are planing to use a pocket program as an axis substitution, the geom needs to be planar. Using a contour for axis sub the geom can be wrapped or planar.

[D&S PRECISION]

Thanks CJeb for replying... if you might have noticed that the pocket is located off the center line in Y+ direction. so here i am trying to use y axis of the machine..as far as i know that i can only use the miil group option when i have my T/C set on Top; and in my case my geometry is not on Top view.So the only option i see that will solve the problem without my satisfying is to set view to Back and use the cross countoring with y axis option ....

[NOTW Programmer]

Thanks CJeb for replying... if you might have noticed that the pocket is located off the center line in Y+ direction. so here i am trying to use y axis of the machine..as far as i know that i can only use the miil group option when i have my T/C set on Top; and in my case my geometry is not on Top view.So the only option i see that will solve the problem without my satisfying is to set view to Back and use the cross countoring with y axis option ....

Screen shot would help.

[CJep]

the pocket is located off the center line in Y+ direction. so here i am trying to use y axis of the machine..as far as i know that i can only use the miil group option when i have my T/C set on Top; and in my case my geometry is not on Top view.

 

You can still program in Mcam TOP, then use transform to index the toolpath to the correct location. When transforming an axis sub toolpath you will use the translate strategy, the distance will be the length of the arc segment.

 

"Screen shot would help."

 

point!

 

CJep

[D&S PRECISION]

Thanks again ...

i am sending you an attached file that will clarify what i meant...

[CJep]

I'm assuming your referring to the closed boundary that is rotated at an angle (looks like somewhere between 9:30 - 10:00).

 

Setup a reference point; I would use the center of the pocket. Create your pocket routine with the geom in the TOP tool/con plane. Use axis sub to wrap the toolpath around the dia. Then use a transform toolpath to index the toolpath to the correct location.

 

You'll also need some reference geom in the right side tool/con plane, vertical 12:00 and a line that represents the current angle of the pocket. Break the arc between 12:00 and your angle. The length of the arc segment is the translation distance on the Y axis using the translate between points method.

 

[D&S PRECISION]

Hi.......

Yes i am referring to the small circle.. trying to explain how i drew it in following steps:

1. change D-Z plane to XYZ top view and drawing the circle on the top of the big circle.

2. change plane to right view and rotate the small circle -30.0 degrees .

3. create a plane by selecting geometery " small circle"

4. translating the circle 0.375 inch in Y direction.

 

the two lines you see are one for the original location before translating ; and the other is for the current location...

 

i will try to implement your method .

 

 

 

thank you very much

[D&S PRECISION]

Hi again

i am attaching the second view file

[D&S PRECISION]

Onca again i am sending you a simulation shot

[D&S PRECISION]

I need to make like the one shown in the attached file

[crazy^millman]

as far as i know that i can only use the miil group option when i have my T/C set on Top

Well I guess it is time for an education about Mill/Turn I have had upwards of 75 T/P planes with no problem. Swtching between 3+2 to full 5 axis in Mill/Turn with no problem either. The machine has a Y axis and if your post is set-up correct then it should not matter how many T/C planes you have. (Let Make sure you understand a T/C Planes is different that a WCS see Picture) Problem that most people are not aware of is the difference between a X-Y Y axis and a true Y axis machine. A Slant Bed machine gets it Y axis by moving the X and Y to achieve a Y axis move. Not a true Y axis move, but gets it done and close enough to make perfect parts, but not a true one Axis Y move like a milling machine would make. The True Y axis machine like the E series Integrex and Mori Seki NT machines are in all reality a 2 axis lathe with a Mill Machine stuck on top of it. Then the Head moves in B axis direction like a DMU machine, expect there is a lot more travel in B axis. Your example is straight forward so I made an straight forward example using the MPLMASTER post, MD/CD to make it. It is on the FTP in X6_Files. It is called MILL_TURN EXAMPLE.MCX. You will see 8 different T/C planes in the file. Anyone is welcome to this file for teaching purposes.

 

 

Here is the NC-Code from this example file.

 

O0000

(PROGRAM NAME - T)

(DATE=DD-MM-YY - 30-06-12 TIME=HH:MM - 18:54)

(MCX FILE - C:\USERS\RONNINE\DOCUMENTS\MY MCAMX6\MCX\MILL-TURN EXAMPLE.MCX-6)

(NC FILE - C:\USERS\RONNINE\DOCUMENTS\MY MCAMX6\LATHE\NC\T.NC)

(MATERIAL - STEEL INCH - 1030 - 200 BHN)

(POST DEV - IN-HOUSE SOLUTIONS INC.)

(TOOL - 239 - 1/2 FLAT ENDMILL - OFFSET - 239 - DIA. - .5")

G20

(TOOL - 239 OFFSET - 239)

( 1/2 FLAT ENDMILL)

G54

N239 T24139

G19 G98

M23

M90

G0 C90.

M89

G0 X6.5 Y0. Z-3.

G97 S1069 M51

X4.

G1 Y-.125 Z-2.875 F6.42

G3 Y-.25 Z-3. R.125

Y0. Z-3.25 R.25

Y.25 Z-3. R.25

Y0. Z-2.75 R.25

Y-.25 Z-3. R.25

Y-.125 Z-3.125 R.125

G1 Y0. Z-3.

G0 X6.5

G55

M90

G0 C60.

M89

X6.5 Y-.5 Z-3.

X4.

G1 Y-.625 Z-2.875

G3 Y-.75 Z-3. R.125

Y-.5 Z-3.25 R.25

Y-.25 Z-3. R.25

Y-.5 Z-2.75 R.25

Y-.75 Z-3. R.25

Y-.625 Z-3.125 R.125

G1 Y-.5 Z-3.

G0 X6.5

G56

M90

G0 C30.

M89

X6.5 Y-.75 Z-3.

X4.

G1 Y-.875 Z-2.875

G3 Y-1. Z-3. R.125

Y-.75 Z-3.25 R.25

Y-.5 Z-3. R.25

Y-.75 Z-2.75 R.25

Y-1. Z-3. R.25

Y-.875 Z-3.125 R.125

G1 Y-.75 Z-3.

G0 X6.5

G57

M90

G0 C0.

M89

X6.5 Y-1. Z-3.

X4.

G1 Y-1.125 Z-2.875

G3 Y-1.25 Z-3. R.125

Y-1. Z-3.25 R.25

Y-.75 Z-3. R.25

Y-1. Z-2.75 R.25

Y-1.25 Z-3. R.25

Y-1.125 Z-3.125 R.125

G1 Y-1. Z-3.

G0 X6.5

G58

M90

G0 C-80.

M89

X6.5 Y-.5209 Z-3.

X3.9088

G1 Y-.6459 Z-2.875

G3 Y-.7709 Z-3. R.125

Y-.5209 Z-3.25 R.25

Y-.2709 Z-3. R.25

Y-.5209 Z-2.75 R.25

Y-.7709 Z-3. R.25

Y-.6459 Z-3.125 R.125

G1 Y-.5209 Z-3.

G0 X6.5

G59

M90

G0 C-100.

M89

X6.5 Y-1.4959 Z-3.

X3.2961

G1 Y-1.6209 Z-2.875

G3 Y-1.7459 Z-3. R.125

Y-1.4959 Z-3.25 R.25

Y-1.2459 Z-3. R.25

Y-1.4959 Z-2.75 R.25

Y-1.7459 Z-3. R.25

Y-1.6209 Z-3.125 R.125

G1 Y-1.4959 Z-3.

G0 X6.5

G54.1 P1

M90

G0 C-135.

M89

X6.5 Y-1.5009 Z-3.

X3.4073

G1 Y-1.6259 Z-2.875

G3 Y-1.7509 Z-3. R.125

Y-1.5009 Z-3.25 R.25

Y-1.2509 Z-3. R.25

Y-1.5009 Z-2.75 R.25

Y-1.7509 Z-3. R.25

Y-1.6259 Z-3.125 R.125

G1 Y-1.5009 Z-3.

G0 X6.5

G54.1 P2

M90

G0 C-165.

M89

X6.5 Y-1.7424 Z-3.

X3.2779

G1 Y-1.8674 Z-2.875

G3 Y-1.9924 Z-3. R.125

Y-1.7424 Z-3.25 R.25

Y-1.4924 Z-3. R.25

Y-1.7424 Z-2.75 R.25

Y-1.9924 Z-3. R.25

Y-1.8674 Z-3.125 R.125

G1 Y-1.7424 Z-3.

G0 X6.5

M90

G28 U0. V0. W0. H0. M55

M30

%

[D&S PRECISION]

Thanks Crazy for the ton of info provided..

 

i made toolpath that has WCS different from T/C planes as you see in the attached pic "backplot".This is not what i am looking for ;though.I need to make the same pocket shown in the other picture file "i-need-this-one".By the way how i can download "MILL_TURN EXAMPLE.MCX".

[Guest]

Can you share your file?

 

I am trying to wrap my mind around what you are trying to do and it seems to me all the info you need has been provided but something is getting lost.

 

I think at this point, your file is going to be the biggest help for all of us including you

[D&S PRECISION]

Hi JParis

 

 

See the difference between the two pictures provided and you will find what i mean. The pocket is 0.3" offset in Y+ direction of the pocket's plane.........I know how to machine what is in "i-dont-need-this-one" file..

 

Thanks for replying...

[Guest]

I'd still prefer a file.

 

As I said, everything has been provided but something is getting lost.

 

You're not far from In House Solutions, I might suggest you contact them on Tuesday morning

 

Good luck

[crazy^millman]

FTP instructions

 

Please review and download the file I did for you. I have all types of offsets. Please share your file without it everyone is less able to help you solve your issues.

[crazy^millman]

I was thinking about this morning and the hole can be on center line and with circle milling it that would still require a Y axis move. So having the hole offset is not an issue here. A hole is a hole and the axis along the center line is still the axis of that hole.

[D&S PRECISION]

hi Crazy.....

 

i think the output code should be something similar to this one:

 

G19 G98 M45 (notice circular cut in YZ plane "G19"

G0 T0303

G97 S5200 M13

C330.0 (Pocket is located on OD -30.0 degree; our C0.0 is on top of tha part")

M68

X8.0 Y-0.375 Z-0.7399 (Here is the pocket is offset in Y axis "Y-0.375" )

X5.7

G1 X5.1 F26.00 ( Tool coming down into part to depth we need)

 

here comes a bunch of lines that create circular motions "G2 or G3" in plane YZ "G19"

 

G2 Y-0.5101 Z-0.7344 J-0.0904 K0.0681 (as an example)

 

G1 Y-0.4915 Z-1.0734 F31.20

G0 X8.0

G28 V0

G28 U0 W0

M69

M46

M5

[crazy^millman]

Okay are you talking about a whole different thing here? Are you are asking about mapping and using the G68 coordinate shift? That is not the same thing and your post will have to be set-up by the dealer for your specific machine.

Edited July 2, 2012 by Crazy^Millman

[D&S PRECISION]

Lol.... where did you get G69 .

M68 is break the c axis

M69 is unbreak the c axis

 

there is no G69 in the code provided

[robk]

Ron is talking about coordinate system rotation (G68).

Either that or you will need to use TPC (G43._) or possibly Dynamic Offset (G54.2) or just use a tooling ball with a known location.

[crazy^millman]

Sorry now I see M68 and not G68 and M69 and not G69. I have not seen one post about the machine and control that helps tons. I go back to I have provided you with a sample file doing what you were asking. People make mistakes and I am one of them, but to be honest at this point I am done helping you. I can only help them who are willing to help themselves. You want help go to your reseller or maybe someone on here will pick up where I left off. Have a great day.

[D&S PRECISION]

Hi Crazy....

First of all, i thank you for your help and dont be sorry ;we all make mistakes.. i solved problem and i did prove it.So i want to share it.

 

All i did is to rotate the pocket to a position so it is lying on the back plane " view 3". so now i can use pocket toolpath that is in the mill menu after changing T/C to 3.I got similar format to the one posted earlier.