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:

G12.1 Polar Interpolation


Recommended Posts

Morning all,

 

I've been suggested to use G12.1 for hole interpolation - which I have no idea what that is nor have ever used it...

I was wondering if anyone here has and how do I go about programming that?   The code in question is for the Doosan Puma and i've been using C-axis as my output since the part itself is larger than the Y axis travel range...

 

-JD

Link to comment
Share on other sites

Can you section the cuts if you must have Y Axis cutting? I have done that where I can re position the part and get what I need to cut the whole shape if it fits within the Y axis travel, but one these machines you sometimes need to approach with with quadrant programming and not full travel programming. By breaking up the programming into sections then you can machine the complete part.

  • Like 2
Link to comment
Share on other sites
On 10/24/2017 at 5:12 PM, C^Millman said:

Can you section the cuts if you must have Y Axis cutting? I have done that where I can re position the part and get what I need to cut the whole shape if it fits within the Y axis travel, but one these machines you sometimes need to approach with with quadrant programming and not full travel programming. By breaking up the programming into sections then you can machine the complete part.

I do this A LOT on table/head machines.  Mostly a 180 half/half split but sometimes on really big parts in sections to get the part in my work envelope.

Link to comment
Share on other sites

JLW:

On 10/26/2017 at 0:26 PM, jlw™ said:

I do this A LOT on table/head machines.  Mostly a 180 half/half split but sometimes on really big parts in sections to get the part in my work envelope.

Have you tried this on a CNC Lathe for face milling?

 

I did and after looking at the code, it doesn't seem to look right.  I had polar interpolation AND C-axis rotation enabled, the only angle i saw was zero deg.

Link to comment
Share on other sites

Look inside your post...there is many times info about how to set these cuts up

 

#Polar interpolation, G112 canned cycle:
# Polar interpolation is active only for face cutting (Right or Left).
# Use the Caxis/Face Contour toolpath. All paths must start and end at
# the 'C0'location for output to be correct. Chain geometry and set
# mi4 to activate G112 mode!

C_AXIS_G12.zip

Edited by Guest
Link to comment
Share on other sites
1 hour ago, JeremyV said:

JLW:

Have you tried this on a CNC Lathe for face milling?

 

I did and after looking at the code, it doesn't seem to look right.  I had polar interpolation AND C-axis rotation enabled, the only angle i saw was zero deg.

Yes, in a Mazak 550MY.  Works exactly the same.

Link to comment
Share on other sites

I was kinda hoping the Polar interpolation would simply do what I needed at zero deg, 30 deg, 90 deg, and 270 deg without having the X axis go so far below centerline and crashing any adjacent tools since the Doosan turret doesn't allow for large part clearance between stations...

Link to comment
Share on other sites
2 hours ago, JeremyV said:

I was kinda hoping the Polar interpolation would simply do what I needed at zero deg, 30 deg, 90 deg, and 270 deg without having the X axis go so far below centerline and crashing any adjacent tools since the Doosan turret doesn't allow for large part clearance between stations...

Not going to happen. It is trying to solve the solution by cutting the shape with using the control to solve the limits. Problem is what may look good on the screen doesn't equate to reality on the machine. Best way will be to break up into section and piece meal it. Where sometimes just because the machine has certain abilities doens't make it the best choice for doing the work. Other option is to leave stations blank on each side or put turning tools hoping it gives you enough clearance to do what you need.

  • Like 1
Link to comment
Share on other sites
  • 3 weeks later...
1 hour ago, JeremyV said:

I've ran a program 4" away from the part just to see the behavior.  It actually did what simulated in mastercam, much to my surprise.  We went with it with zero issues so I guess thats a plus... for now.  Will continue to keep an eye on that.

Did you have to move holders around to allow for that to work or was there enough room to not hit like you originally said it would? Thanks for the update.

Link to comment
Share on other sites
On 01/11/2017 at 10:11 AM, jlw™ said:

You can also set WCS and offsets in the machine to resolve the angles you want.  Just another way.

Complementing the suggestion above, you can just play with the current work offset rotary value via program... 

Something like (Pseudo code)

#54005 - > Internal control  variable holding current C axis value of G54 offset 

G54

#1000=#54005 ;Backup original C value from work offset table on variable #1000

Your toolpath here...  

#54005=#54005+90 ;Increment G54 C current value by 90 degrees 

G54 ;Re-read G54 offsets 

Repeat your toolpath... 

#54005=#54005+90 ;Increment G54 C value by 90 degrees again 

G54 ;Re-read G54 offsets

Repeat your toolpath... 

#54005=#1000 ;Restore your original C value on G54

Blablabla... 

You can use conditional logic to improve my pseudo code written on a cellphone while a take a xxxx... :lol:

  • Like 1
Link to comment
Share on other sites

I could never program circular interpolation on a NAKA MURA TMC15 WITH FANUC OTC CONTROL .  The control needed the proper parameter for G107 or G112. It was requested many times but big bosses (government bureaucrats) did not know what we were talking about and it never happened. Arcs had to be broken into small segments, but the control memory could not take more than 19K  and  long programs had to be sectioned into small programs and fed one by one to the control.

 

John

Link to comment
Share on other sites
On 11/17/2017 at 4:25 PM, C^Millman said:

Did you have to move holders around to allow for that to work or was there enough room to not hit like you originally said it would? Thanks for the update.

Did not have to move anything.   The Y axis does not move for polar interpolation.  Every hole was done at "X+" location, which was where I wanted them to be.  Plus programs are so much shorter now.

Link to comment
Share on other sites
5 hours ago, JeremyV said:

Did not have to move anything.   The Y axis does not move for polar interpolation.  Every hole was done at "X+" location, which was where I wanted them to be.  Plus programs are so much shorter now.

Drill holes is much different that cutting a kidney slot or something of that nature is what I was envisioning. Yes drilling holes is just a matter of using the C Axis process or setting up the correct planes and you are off to the races. Glad you got it figured out and thank for posting back up it is nice to know when someone has been helped.

  • Like 1
Link to comment
Share on other sites
9 minutes ago, C^Millman said:

Drill holes is much different that cutting a kidney slot or something of that nature is what I was envisioning. Yes drilling holes is just a matter of using the C Axis process or setting up the correct planes and you are off to the races. Glad you got it figured out and thank for posting back up it is nice to know when someone has been helped.

No problem.

I'll reply here if I run into any issues with irregular shaped objects... I kinda want to try that and see what happens.

 

Thanks all.

-JD

Link to comment
Share on other sites
  • 8 months later...

I'm currently not seeing the results I'd like with the G12.1. Attached is the current code (Citizen L20-Mitsubishi control) and the blueprint. The print is in inches but the program is in metric. I programmed the final part dimension + the radius of the tool (.125"), this way the R value on the offset screen is 0.  
The issues are as follows, the final dimension is approximately .032" to big on the .072" +0./-.004" dimension(width across flats). I've programmed the X and C axis radially. I verified that the tool is centered (X0./Y0.) to the sub-spindle.
Also, there's no .127mm(.005") radius on the corners of the square. 


As the program reflects I'm using G41 and G2's. Per the attached picture captured from the Instruction Manual for the Citizen L20, I should be using G42 and G3's, which is correct? I'm wondering if this is why my part has no .127mm(.005") radius on the corners of the square? 

Thanks in advance for the support.

300.txt

FSP.PNG

G41-G42.PNG

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...