Loïc19962

Mastercam Lathe

Recommended Posts

is it possible to create a taper on Mastercam to avoid the error on the lathe, sorry for my English ?

Share this post


Link to post
Share on other sites

You should have a taper adjustment in the tool menu.

Share this post


Link to post
Share on other sites
5 hours ago, Machineguy said:

You should have a taper adjustment in the tool menu.

yea if you have an option on your machine i would also do it at the controller, so that way you dont have to go back and forth between mastercam and the machine as tools wear, etc. 

some lathe machine controllers have taper control options built right in to handle taper on parts, consult your machine dealer or manual to see if your controller has this option and in my opinion that would be the best solution, but it can certainly also be done in mastercam i just think it would be easier on the operator at the machine control.

Share this post


Link to post
Share on other sites

You can do it on MC, easiest way is to draw a line at the angle you need to fix, and make a single pass operation.  Then if you need to adjust it further at the machine, just change  either the beginning or ending X coordinate.

Share this post


Link to post
Share on other sites

On a lathe i would just add a U command equal to the taper error. Run part with offset in X (so you don't scrap the first piece). Measure part for taper error. Look in code for the line with the G01 Z-where ever and put the U on that line.

Eg;

G01 Z-1.3125 U.002

The U will move the X axis incrementally that value over the length of the Z move. I would try to figure out where the problem is. Poor set up (to much stick out comes to mind), need center support, or previous crash causes taper at all times. IMHO best to fix the problem than to try and work around.

  • Like 4

Share this post


Link to post
Share on other sites
8 hours ago, Allan said:

On a lathe i would just add a U command equal to the taper error. Run part with offset in X (so you don't scrap the first piece). Measure part for taper error. Look in code for the line with the G01 Z-where ever and put the U on that line.

Eg;

G01 Z-1.3125 U.002

The U will move the X axis incrementally that value over the length of the Z move. I would try to figure out where the problem is. Poor set up (to much stick out comes to mind), need center support, or previous crash causes taper at all times. IMHO best to fix the problem than to try and work around.

Hey, that's a new one on me.  Never tried that.  What all controls have you done this on?

Share this post


Link to post
Share on other sites
3 minutes ago, jlw™ said:

Hey, that's a new one on me.  Never tried that.  What all controls have you done this on?

Fanuc and HAAS controllers both have separate incremental letters assigned for each axis, X=U, Y=V, Z=W. so there is no need for G90/G91 as with a mill.

I cant speak for other controllers.

Share this post


Link to post
Share on other sites

I think he's using Mazatrol. If so, change it from line to taper in the program. 

Share this post


Link to post
Share on other sites

I think he's using Mazatrol. If so, change it from line to taper in the program. 

Share this post


Link to post
Share on other sites

I think he's using Mazatrol. If so, change it from line to taper in the program. 

Share this post


Link to post
Share on other sites

I'm not sure, but if it's Maza-troll, you can change it from line to taper in the program.

:D

Share this post


Link to post
Share on other sites
3 hours ago, AHarrison1 said:

Fanuc and HAAS controllers both have separate incremental letters assigned for each axis, X=U, Y=V, Z=W. so there is no need for G90/G91 as with a mill.

I cant speak for other controllers.

Okuma has it too, of course.

Mostly use it in threading canned cycles. cant remember if it's an I or a Q off the top of my head, but the sign designates direction. (ie smaller of bigger towards the chuck)

Share this post


Link to post
Share on other sites

All of these ideas will work, I like the U value the best may I add that if you would put a variable in the U address you could make it adjustable and you could adjust the variable if any more adjustments were needed and not have to edit the program and allow  the operator to make his own adjustments. example U#510 then just put the adjustment amount in register 510. 

Share this post


Link to post
Share on other sites
7 hours ago, AHarrison1 said:

Fanuc and HAAS controllers both have separate incremental letters assigned for each axis, X=U, Y=V, Z=W. so there is no need for G90/G91 as with a mill.

I cant speak for other controllers.

Learn something new everyday!  Ive run Haas lathes for 13 years and never knew!  Thanks!

Share this post


Link to post
Share on other sites

I can't think of any controls that don't have UVW incremental in lathe.  What I did not know is that you can use it on the same line.

Share this post


Link to post
Share on other sites

I used U all the time with Fanuc 18i. It is ok when turning from one point to another, but I hated it when some people used it for multi point correction when turning long shafts instead of absolute X values.

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us