Printable View
hi there,
We are trying to thread mill 1/8 - 27 NPT on a 5-axis lathe. Most of the software out there would only output code for a machining centre. Our lathe will only accept J & K. XYZ axis on a mill but on a lathe X (diam) is the tool axis. Any help would be appreciated.
Thanks in Advance
HI there -
I'm having a hard time myself understanding this thread mill business.
But in a lathe why not G76 thread cycle...just wondering.
Cheers
Jorge
Which axis is the thread rotating around?Quote:
Originally Posted by Jr. Programmer
EDIT: Silly me you mentioned it X is the tool axis you say.
I don't use software but this should be possible. Get your code output which has X, Y, Z, I and J and then do a Find and Replace in a word processing program:
Z will become X
X will become Z
Y stays the same
J stays the same
I becomes K
Your tool is moving in the Y, Z plane and advancing along the X axis. (I think)
I believe G76 thread cycle would be used for ID threading of a cylindrical part. I need to thread mill perpendicular to the the z-axis (ie. the top of the part).
hi Geof,
I hear ya..but on a lathe X is the diametrical which means (Z x 2 in diameter). Having said that, does the J and K change accordingly? If so how much? These machines are not quite simple as a 3 axis mill...
No not quite as simple :) .Quote:
Originally Posted by Jr. Programmer
I don't think this would have any effect on J and K and it could be as simple as using a G code to shift the X axis from diameter measure to radius measure. If I was designing a machine that could turn and mill I would incorporate this feature.
If there is no way to command this then you might have to generate your code using twice the pitch so when you swap the Z and X you have compensated for it.
Also if you are just using three of the axes and they are orthogonal then you have a three axis machine.
In theory you can Interpolate a Helical Thread on a 5 Axis Lathe. But you need a true Y and C Axis to do this. Also you will need to find the G-Code Designation that will Synchronize the C Axis with the Y Axis. What this will do is replace the Y Axis with the C Axis. Maybe a G100, G101, G120, G121, G200, G201, G300, or G301. You may also have to Designate a Work Plane.Quote:
Originally Posted by Jr. Programmer
This is still a 3 Axis movement but in the C, Z, and X Axies. It is the Same as an XYZ Movement but you are substituting the Y for the C and the X is now your Depth in the part.
What Machine, and Control Are you trying this on??
I have done this once before on a Nakamura-Tome. I will try to find the Program so you can see it.
G76 to my knowledge is only used for the XZ Plane, G18.
G90 G19
S6853 M3
G00 C0.000 Y0.0000 Z0.0000 X0.0787 Position to centerline of thread/ 0.0787 above surface
G91 - incremental
G00 X-0.3692
G41 G01 Y0.000 Z-0.1555 F39.0640
G03 Y0.000 Z0.3480 X0.0185 J0.000 K0.1740 F3.5304
G03 Y-0.1928 Z-0.1925 X0.0093 J-0.0001 K-0.1926 F7.5084
G03 Y0.1928 Z-0.1931 X0.0093 J0.1929 K-0.0001
G03 Y0.1934 Z0.1931 X0.0093 J0.0001 K0.1932
G03 Y-0.1934 Z0.1937 X0.0093 J-0.1935 K0.0001
G03 Y0.000 Z-0.3492 X0.0185 J0.000 K-0.1746
G40 G01 Y0.000 Z0.1555
G00 X0.2952
G90
This should produce a 1/8 npt in you machine.
Hope it will be of any help...
Quote:
Originally Posted by tobyaxis
On machines equipped with FANUC controls G12.1 allows you to use the C axis as the Y where you are using polar interpolation to cut your part. the only problem with using G12.1 is you have to be in G1 mode at all times no G0 is allowed in your tool paths. all positioning have to be done in G1 mode. G18 plane should be active to use G12.1. the other problem using G12.1 is you have to cut at X0.