HELP post quiston

[rex miller]

I got a new machine. A romi 20 x 60 lathe.

I have 2 post for the romi.

but i need to change the x value from a positive

to a negitive. to run right.

Im just learning MC lathe. any help to show how

to change this is verry thankfull.

[crazy^millman]

Look in the post for a switch. I know this has been covered on the Mori-Seki do a search and see if that appiles to this.

 

HTH

[rex miller]

I tried to change it in the offsets page

but it still post in positive x..

I checked my lathe (romi) to see how it

looked in the G-code. and it is positive!

But my tools work from the bottom or

operator side.

os i may be asking the wrong quiston.

master cam shows tools working from the top.

can i change this to what my lathe does.

this cnc is a flat bed lathe.

runs like a manual ...

thanks

[Bzwak]

Have you tried setting the tool parameters up differently? Select the bottom side orientation.

[crazy^millman]

I still think it is just a post issue may have to wait till Monday to contact you dealer and see if they can help you if no one comes up with an answer for you.

 

HTH

[jimspac]

You can also change D+ to D- by clicking on CPLANE +DZ>Next Menu> -DZ. That will change your coordinate system to negative X

[Guest]

Look for this line in your post.

 

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

 

change the sign of the number.

[Ian q]

Will changing x to neg. also change G2 to G3 and visa-veras?

Ian

[GxHxOxSxT]

hi rex,

post may be the easiest fix, however if you draw all parts on the plus side of x-axis you can xform rotate about the z axis and copy(will give you a full view of the part) then chain your tool path on the neg.(or operators) side and double click on the tool you are using, in the top right corner click on set up tool, change turret from top to bottom, and it will post with neg. x values.

 

hope this helps

Rob

[?Mark]

+1 to Mark

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

 

Also you will need to change the following:

 

sg02 G3 #Circular interpolation CW

sg03 G2 #Circular interpolation CCW

 

 

This will address Ian q's concern about correct G2 G3 codes.

If you want to change existing nc file to run on a lathe with opposite x axis there is a cool vb script on ftp that does this, courtesy of Roger Martin.

Hope it helps

Kind regards, Mark