Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Haas fanuc lathe post edit - G97 Rpm and G50 Max


Recommended Posts

I am editing my Haas lathe post so my labels are on top  - I can do mill post edits just fine but lathe seems to have more variables

I want to understand how can I set my first G97 RPM to not be such a high number ( if I am using G96 CSS).   I would like a default like G96 S500 - I understand in drilling I would want a higher number but I don't know where the random number comes from

ex:

G97 S2247 M03 ( where does this S# come from ?)

G0 G54 X1.7 Z.03 M08

G50 S3000

G96 S1000

 

also want to where can I rest the max number on G50 - I seem to be set at 3600 but I don't know where that setting is - If I go below 3600 it will change - if I set it to 4500 it will max out at 3600. I cant find in control or machine def.

thks

 

 

Link to comment
Share on other sites

It usually helps if you tell people what version of mastercam you're on.  If you're paying for maintenance your rep should be able to help you easily.  Have you talked to them yet about this?  

 

Quote

G97 S2247 M03 ( where does this S# come from ?)

This number is calculated out from your SFM.  

1000 SFM * (12/pi)  /  1.7" Diameter = 2247 RPM

 

So it kicks on the spindle at the correct speed for your SFM at your first positioning move.  This number is also limited to your max spindle speed.  

 

Link to comment
Share on other sites

Thanks for response - So it calculates largest diameter machined @ 1000sfm. I  was doing Cam instructor lathe course and I think stock used was 1.500". Any way I didn't know if I had any control to force a G97 RPM if going to use G96. 

any thoughts on the cap for max speed - because I had a default at 10000 and I ended up with 3600 - so I played with it and some setting must have it maxed but I cant find it. 

 

I teach using Version X9 & 2017  and also have 2018.  I am an educational buyer so support is not as comprehensive.  I do know many people in Seattle where the Education office but I thought this forum would be a good resource as well.  I am a do it yourself type.

 


 

Link to comment
Share on other sites

Due to a large portion of people pirating the software, people here are a bit hesitant to give out information on post editing.  If you're familiar with working on the post for the mill, i'll give you a hint.  Max speed in found in the post,  you should be able to find it pretty quickly. 

 

I don't think there is any way to control it directly in the program as it sits now,  but you can edit the post to do whatever you want it to do.  You can add a modifier or just hard code a static number instead of the variable.  Lots of ways to skin a cat on that one. 

 

Quote

So it calculates largest diameter machined @ 1000sfm. 

not quite, but pretty close.  It calculates the rpm it at whatever the first positional movement is.   Thats why a boring bar would start faster than an OD turn tool.  

Link to comment
Share on other sites
On ‎7‎/‎5‎/‎2018 at 1:41 PM, soymilk said:

Due to a large portion of people pirating the software, people here are a bit hesitant to give out information on post editing.  If you're familiar with working on the post for the mill, i'll give you a hint.  Max speed in found in the post,  you should be able to find it pretty quickly. 

 

I don't think there is any way to control it directly in the program as it sits now,  but you can edit the post to do whatever you want it to do.  You can add a modifier or just hard code a static number instead of the variable.  Lots of ways to skin a cat on that one. 

 

not quite, but pretty close.  It calculates the rpm it at whatever the first positional movement is.   Thats why a boring bar would start faster than an OD turn tool.  

Thanks on that.  I am aware of some pirating I have seen at some companies but one I know got caught.  Now that I am in education - I probably could get help from that division but like I said I am a do it your self guy. I used to modify all posts for our Smartcam system at our NH company with many machines,  thanks

Link to comment
Share on other sites

The Max SS value is set in the Operation itself. Just like the CSS value.

This allows you to set different 'max' values, for each Operation. For example, you might want G50 S3600 for an OD roughing Op, but for Parting off the workpiece, you might want to set G50 S800 (to prevent damage or chip wrapping).

The 'direct RPM start' is handled by a switch inside the Post Processor. This switch allows you to turn on/off the output of:

G97 Sxxxx M03

Prior to the G96 Sxxxx.

I always recommend setting up your Post so that the 'Max Spindle Speed Clamp' command is output before the G96 Sxxx. Otherwise you are using whatever the 'last' setting was.

One of our members 'Gcode' has a story about a big VTL, and the operator deleting the G50 S150 (because he didn't know what it was for). Then the control hit the G96 S400 line, and threw the part off the lathe, almost killing the operator.

Since you are going to be the instructor, make sure you know what those codes do, and that your students do also...

 

  • Like 1
Link to comment
Share on other sites
11 hours ago, Colin Gilchrist said:

The Max SS value is set in the Operation itself. Just like the CSS value.

This allows you to set different 'max' values, for each Operation. For example, you might want G50 S3600 for an OD roughing Op, but for Parting off the workpiece, you might want to set G50 S800 (to prevent damage or chip wrapping).

The 'direct RPM start' is handled by a switch inside the Post Processor. This switch allows you to turn on/off the output of:

G97 Sxxxx M03

Prior to the G96 Sxxxx.

I always recommend setting up your Post so that the 'Max Spindle Speed Clamp' command is output before the G96 Sxxx. Otherwise you are using whatever the 'last' setting was.

One of our members 'Gcode' has a story about a big VTL, and the operator deleting the G50 S150 (because he didn't know what it was for). Then the control hit the G96 S400 line, and threw the part off the lathe, almost killing the operator.

Since you are going to be the instructor, make sure you know what those codes do, and that your students do also...

 

Thanks - been teaching for 5 years now but good advice for all. In industry, back in the manual G Code days, we always had a format in each shop.  On the lathe I like to have a G28 as first line - to send it home before tool change. As a setup guy for 30 years I have to rerun tools etc. So I want programs to have everything in place for me or other users. So that functions will be automated and won't have to remember everything and reduce or eliminate that dreaded crash.  So on a Lathe or Mill I know what I want for code and now just getting Mcam to spit it out.  I sometimes have to accept what I get but I always try to tweak.

Lathe

G28

T101

G97 S500 (I call this just get it spinning - always a slow RPM)

G50 S3750 (Rev limiter)  ( Ps: there is a Post setting for this also - max number - I had S10000 and it would only post S3600 - until I changed per above posts)

G54 G00 X1.1 Z.1 M8

( Now its time to decide what to do )

G96 S1000 ( except if its drilling or threads)

yada yada

M9

G28

M01

 

 


 

Link to comment
Share on other sites
41 minutes ago, cncdude5x said:

  I sometimes have to accept what I get but I always try to tweak.

 

That's why this forum exists. You don't have to accept it, unless the code is exactly how you want it to be formatted.

In general, if there is a will, there is a way to get it done in the Post. I started modifying Posts just like you. Messing around until I figured out how to get what I wanted.

Then I got a real education in how the MP Post Language works, and have been some pretty trick Post work ever since...

Link to comment
Share on other sites
13 hours ago, Colin Gilchrist said:

That's why this forum exists. You don't have to accept it, unless the code is exactly how you want it to be formatted.

In general, if there is a will, there is a way to get it done in the Post. I started modifying Posts just like you. Messing around until I figured out how to get what I wanted.

Then I got a real education in how the MP Post Language works, and have been some pretty trick Post work ever since...

ha  - what I meant about accepting was knowing the program will work but time not allowing me to fix at that moment.  I've had cranky bosses in hurry up mode when I 'm also trying to deal with issues. Like the time we weren't getting a 4th axis A position at the top of every tool chg.  It bit someone on a rerun.  machined the wrong rotation

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...