Lathe Question

[FITIN IRISH]

I am programming a Haas Lathe TL 2. The problem I am having is that all of my X moves are negative how do I make them positive? The tool motion is ok.

 

Thanks

[Guest]

HAve you checked in your post under

 

MAchine specific settings?

 

code:

---

dia_mult    : 2     #Multiplier for output on X axis (Neg. switches sign of X)

---

[Hymen]

You need to go into your post and find this area:

and use switch sign from basic

#Machining position turret/spindle settings

# Switch strings based on turret position top/bottom-left/right and cut type.

# Turret position is based on the Mastercam settings (see lathtype).

# Strings are re-assigned for output in the routine psw_str_mult.

# The string variable sw_string holds the place position value to determine

# how to assign the strings. Planes are relative to the view from Mastercam.

# Assign the 17 digit string following the alpha columns below:

# A - C axis, 1 = axis winds, 2 = axis signed, 3 = indexer

# B - Spindle direction, 0 = normal, 1 = reverse

# C - Plane 0 arc/comp, 0 = normal, 1 = switch

# D - Plane 1 arc/comp, 0 = normal, 1 = switch

# E - Plane 2 arc/comp, 0 = normal, 1 = switch

# F - Plane 0, 0 = G17, 1 = G19, 2 = G18

# G - Plane 1, 0 = G17, 1 = G19, 2 = G18

# H - Plane 2, 0 = G17, 1 = G19, 2 = G18

# Decimal (required)

# I - Plane 0, X axis, 0 = normal, 1 = switch sign from basic

# J - Plane 0, Y axis, 0 = normal, 1 = switch sign from basic

# K - Plane 0, Z axis, 0 = normal, 1 = switch sign from basic

# L - Plane 1, X axis, 0 = normal, 1 = switch sign from basic

# M - Plane 1, Y axis, 0 = normal, 1 = switch sign from basic

# N - Plane 1, Z axis, 0 = normal, 1 = switch sign from basic

# O - Plane 2, X axis, 0 = normal, 1 = switch sign from basic

# P - Plane 2, Y axis, 0 = normal, 1 = switch sign from basic

# Q - Plane 2, Z axis, 0 = normal, 1 = switch sign from basic

What John said.

[gcode]

Jerry

when you program your cuts, are your tools pointing up from the bottom of the screen , or down from the top? Down from the top is the way most posts and X machine/control definitins are set up.

If you are doing it this way and still getting

-X gcode, there is something wrong with your

Machine Definition.

Go to Help and run a zip2go of a file that's giving you trouble. Email it to me or upload it to the ftp site and I'll take a look at it

[FITIN IRISH]

Thanks so much guys for all the help. My tools are pointing up from the bottom of the screen.

[gcode]

quote:

---

My tools are pointing up from the bottom of the screen

---

Jerry that is the X- side of the machine and

things are working as they should.

 

Try running a toolpath from the top

[Hymen]

+1 gcode

[FITIN IRISH]

The Machine is a Haas toolroom Lathe. X minus will not work.

[gcode]

quote:

---

X minus will not work.

---

I know, but X+ is from the top so you have to program that way.

An OD tool should backplot with the tip down

towards the bottom of the screen and the shank towards the top.

Your cutting geometry should be drawn above

X zero, not below.

If you do it this way you will get X+ output

[FITIN IRISH]

I got it to work when I changed my post as suggested "dia_mult from 2 to -2.

 

Many thanks to all of you.

[dan m]

jerry

I think what gcode was trying to say is click on planes at the bottom of the screen than click on lathe diameter than click on x+ z+.

It sounds like you have x- z+ selected

[FITIN IRISH]

Thanks Dan, I will try that. I have not used the Lathe module in years,mostly mill. Do you know how I can change my post to output R(radius values) instead of I and K.

[dan m]

Jerry

you will have toi change your post back to where it was originally for that to work. to change the post from i&k there are some questions at the beginnig of the post and it should be in there. I'll look when i get home.

 

hth

[dan m]

Jerry

are you useing mcx?

[MCFELIX]

you can tell the hass company to change a parameter to work viceverse

[Jayson Kramer]

Jerry were you working?

[FITIN IRISH]

I am using MX2. Jay I am in Valencia,CA

[Don S at Barefoot CNC South]

Jerry you have mail

[dan m]

to change i&k to r in your machine groups click on the file box then the edit box then contol def at the top.and on the right side you will see arc as 1 of the choices. just chance the arc center type to rad. hth