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:

4 Axis Lathe - Polar Interpolation G12.1 for Off-Center Holes


Recommended Posts

Hello eM,

Polar interpolation is used on lathes that have a C-axis, but not a Y-axis. To interpolate a shape on the face of a part for example, polar interpolation converts XY corrdinates into their equivalent XC coordinates.

It works like a canned cycle:

G12.1 (polar on)

... code goes here

G13.1 (polar off)

 

It appears that polar interpolation does not work with off-center ID holes, such as a bolt circle.

If an ID hole is on the center-line of the part as shown in the first picture, the machine can move in X and spin the C-axis 360 degrees to complete a full diameter shape.

However if the hole is off-center as shown in the second photo where the tool moves to the left, the machine can move in X, but cannot rotate 360 degrees to complete a full diameter shape. It appears that it can only rotate 180 degrees, and would then have to rotate the C-axis 180 degrees in the opposite direction to complete a full diameter shape. This leaves xxxxty finishes inside holes.

Is it wrong to state that polar interpolation cannot do full circles on holes that are off-center, such as a bolt circle? Or least state that it is not very good at it, and will not create clean circular shapes?

 

polar_interpolation_question_0.png

polar_interpolation_question_1.png

Link to comment
Share on other sites
On 10/16/2020 at 5:45 AM, mayu said:

Hello eM,

Polar interpolation is used on lathes that have a C-axis, but not a Y-axis. To interpolate a shape on the face of a part for example, polar interpolation converts XY corrdinates into their equivalent XC coordinates.

It works like a canned cycle:

G12.1 (polar on)

... code goes here

G13.1 (polar off)

 

It appears that polar interpolation does not work with off-center ID holes, such as a bolt circle.

If an ID hole is on the center-line of the part as shown in the first picture, the machine can move in X and spin the C-axis 360 degrees to complete a full diameter shape.

However if the hole is off-center as shown in the second photo where the tool moves to the left, the machine can move in X, but cannot rotate 360 degrees to complete a full diameter shape. It appears that it can only rotate 180 degrees, and would then have to rotate the C-axis 180 degrees in the opposite direction to complete a full diameter shape. This leaves xxxxty finishes inside holes.

Is it wrong to state that polar interpolation cannot do full circles on holes that are off-center, such as a bolt circle? Or least state that it is not very good at it, and will not create clean circular shapes?

 

polar_interpolation_question_0.png

polar_interpolation_question_1.png

I've done stuff like that with without problems. One of the biggest issued i had with the post for the Haas was i had to turn of the machine to break arcs at quadrants. The control got confused when trying to do complete circles when it was one big arc.

  • Like 1
Link to comment
Share on other sites
On 10/19/2020 at 10:48 AM, Rocketmachinist said:

I've done stuff like that with without problems. One of the biggest issued i had with the post for the Haas was i had to turn of the machine to break arcs at quadrants. The control got confused when trying to do complete circles when it was one big arc.

Yes when using polar with off-center-holes, for obvious reasons, you cannot rotate the c-axis 360 degrees in a single pass when a tool is inside a hole.

Therefore you cannot cut all four quadrants in a single pass.

You have to enter a quadrant - back off - re-position - enter again - rinse and repeat.

This approach does not leave clean circular finishes inside holes, is painful with deep holes, and requires complex post edits.

Sending a reamer through a hole is a lot simpler and cleaner.

 

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

Yes when using polar with off-center-holes, for obvious reasons, you cannot rotate the c-axis 360 degrees in a single pass when a tool is inside a hole.

Therefore you cannot cut all four quadrants in a single pass.

You have to enter a quadrant - back off - re-position - enter again - rinse and repeat.

This approach does not leave clean circular finishes inside holes, is painful with deep holes, and requires complex post edits.

Sending a reamer through a hole is a lot simpler and cleaner.

 

I've never had to do it the way you said. I just changed my control def to "Break arc at quadrants"

Link to comment
Share on other sites
On 10/24/2020 at 8:15 PM, mayu said:

Pretty sure we're talking about the same thing.

On a C-axis lathe with no Y, you cannot interpolate an off-center circle in a single pass.

Instead you cut one quadrant at a time, breaking the arc at each quadrant.

 

1831956985_breaarcsmill.thumb.PNG.5b7305d3ce59e513a98d7e179b071452.PNG

Check these settings and then use your toolpaths like normal, you shouldn't have to make 4 toolpaths for one hole. One will work. Your machine and post should handle it fine if you make these changes.

Link to comment
Share on other sites
On 10/26/2020 at 8:43 AM, Rocketmachinist said:

1831956985_breaarcsmill.thumb.PNG.5b7305d3ce59e513a98d7e179b071452.PNG

Check these settings and then use your toolpaths like normal, you shouldn't have to make 4 toolpaths for one hole. One will work. Your machine and post should handle it fine if you make these changes.

Thanks for the response.

Yes you are correct - it is not necessary to make multiple toolpaths, but it is still physically impossible to cut an off-center hole in a single pass without a Y axis.

Instead the toolpath will have to cut different sections (quadrants) of the hole until the hole is complete.

You can still cut a hole, but getting a clean circular finish is another story.

With small deep holes (under 5mm), it gets even more difficult.

Everytime the toolpath approaches a different section of the hole, it generates entry/exit moves, initializes cutter-comp, etc., depending on your application.

On most Fanuc controls, there can be no G00 moves in the polar-interpolation canned cycle, so getting a satisfactory toolpath can be a real pain in the neck.

Sometimes reamers are easier.

Link to comment
Share on other sites
45 minutes ago, JParis said:

Unless I am mistaken, a C-Axis Face Contour should do exactly what you need...C & X motion only

Correct - but it will not cut the hole in a single pass - that's the issue.

If the hole is on center you can do it in one pass - you move in the positive X direction and spin the spindle 360 degrees.

For off-center holes, such as bolt-circles, it's a different animal.

If you're inside of a bolt circle hole for example, and you rotate the spindle 360 degrees, you end up with a circular slot on the face of the part.

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

Correct - but it will not cut the hole in a single pass - that's the issue.

If the hole is on center you can do it in one pass - you move in the positive X direction and spin the spindle 360 degrees.

For off-center holes, such as bolt-circles, it's a different animal.

If you're inside of a bolt circle hole for example, and you rotate the spindle 360 degrees, you end up with a circular slot on the face of the part.

If the tool is not perfectly on center and aligned correctly in the machine then yes I would expect that to happen. When is the last time you checked the center of the tool to the center of the spindle?

Link to comment
Share on other sites

I dunno I bo bolt holes on my Haas all the time with milling. This code is read by my 2001 SL20 all the time.

%
O0000
(T)
(DATE=DD-MM-YY - 28-10-20 TIME=HH:MM - 14:46)
(MCX FILE - T)
(NC FILE - C:\USERS\ASMURPHY\DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\LATH...\T.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 234 OFFSET - 234)
( 3/16 FLAT ENDMILL)
T23634
M154
G97 P2852 M133
G98
G112
G17
G00 G54 Z.25 Y0.
X1.1796
Y1.4381
Z.1
G01 Z-.1 F6.16
G02 X1.1934 Y1.4049 R.0469
X.8405 Y1.052 R.3529
X.4876 Y1.4049 R.3529
X.8405 Y1.7578 R.3529
X1.1934 Y1.4049 R.3529
X1.1793 Y1.3063 R.3529
X1.1568 Y1.2783 R.0469
G00 Z.25
G113
G18
M155
M135
G53 X0.
G53 Z0.
M30
%

 

717113568_facecontour.thumb.PNG.d346617e4f0a82c35b469586384f100d.PNG

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

I dunno I bo bolt holes on my Haas all the time with milling. This code is read by my 2001 SL20 all the time.

Thanks for sharing.

As I mentioned, I'm referring to machines that do not have a Y axis.

The code you've posted is using X and Y coordinates.

Pretty sure you don't need to use G112 in this situation - you can just interpolate like you would on a mill in the G17 plane.

Polar interpolation converts X Y coordinates into X C coordinates.

When you're using X and C, the C axis compensates for the lack of a Y axis.

It's hard to visualize.

Link to comment
Share on other sites
12 hours ago, mayu said:

Thanks for sharing.

As I mentioned, I'm referring to machines that do not have a Y axis.

The code you've posted is using X and Y coordinates.

Pretty sure you don't need to use G112 in this situation - you can just interpolate like you would on a mill in the G17 plane.

Polar interpolation converts X Y coordinates into X C coordinates.

When you're using X and C, the C axis compensates for the lack of a Y axis.

It's hard to visualize.

My Sl20 doesn't have y axis. I'm using g112 polar interpolation it creates a way smoother path than using XC alone and with way less lines of code.

Link to comment
Share on other sites
1 hour ago, Rocketmachinist said:

My Sl20 doesn't have y axis. I'm using g112 polar interpolation it creates a way smoother path than using XC alone and with way less lines of code.

Hmm...interesting.

Does the C axis rotate during these operations?

It seems like there would have to be some C axis rotations. Perhaps your G112 canned cycle completely overrides it.

Our C axis machines will not take Y axis moves or G17 plane commands.

Looks like your machine takes both.

Link to comment
Share on other sites
1 hour ago, mayu said:

Hmm...interesting.

Does the C axis rotate during these operations?

It seems like there would have to be some C axis rotations. Perhaps your G112 canned cycle completely overrides it.

Our C axis machines will not take Y axis moves or G17 plane commands.

Looks like your machine takes both.

Yes C axis rotates like any normal Polar interpolation would. G17 is XX plane and G18 is XZ and G19 is YZ when calling arcs. They are not needed for any other machining expect when calling a G02, G03, G12, G13, G112 or G113. You post should be defining it correctly. 

Have you checked to make sure the live tooling is on center line correctly? Yes they can be off and yes it make a huge difference when doing things like this. Simple drilling and other things it will be off and still make a part that can pass inspection, but you do what your doing and any deviation is going to be compound and show up. 

Link to comment
Share on other sites
21 minutes ago, crazy^millman said:

Yes C axis rotates like any normal Polar interpolation would. G17 is XX plane and G18 is XZ and G19 is YZ when calling arcs. They are not needed for any other machining expect when calling a G02, G03, G12, G13, G112 or G113. You post should be defining it correctly. 

Have you checked to make sure the live tooling is on center line correctly? Yes they can be off and yes it make a huge difference when doing things like this. Simple drilling and other things it will be off and still make a part that can pass inspection, but you do what your doing and any deviation is going to be compound and show up. 

So even though there are no C axis rotations in the code shown above, the machine is rotating the C axis and performing those calculations in the background?

In the code above, you wouldn't see the C axis rotations in the monitor while the machine is running - only X and Y moves?

This is different from what our technician showed us.  On our machines the G12.1 canned cycle generates all X and C moves, will not take Y moves, and will not take any plane other than G18 (XZ).

Again these machines do not have a Y axis.

Link to comment
Share on other sites
7 hours ago, crazy^millman said:

We have not established you machine or control. How about we do that before doing anything else.

Hi Crazy^millman,

This began as a general discussion about using the G12.1 or G112 polar interpolation canned cycle for off-center holes, such as bolt circles.

This thread pertains specifically to C axis lathes that do not have a Y axis.

Regardless of the machine, it is not possible to rotate the C axis 360 degrees while the tool is engaged in a bolt circle hole without cutting through the side of the hole and creating a circular slot on the face of a part.

See the photos above that have 4 holes on the face of the part. Imagine if the tool was inside one of those holes, and the C axis rotated 360 degrees.

Instead the tool must cut small sections of the hole by utilizing the X and C axes simultaneously, until the hole is complete.

The core argument was that it doesn't leave nice finishes, and is a painful procedure with small, deep holes when factoring entry/exit moves and cutter comp initialization.

The code that Rocketmachinist shared sparked a tangent conversation about using Y coordinates on machines that do not have a Y axis.

Apparently Rocketmachinist can enter Y coordinates inside of the G112 canned cycle without getting any alarms, even though his machine has no Y axis.

I was unaware that a machine without a Y axis could do this.

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

Hi Crazy^millman,

This began as a general discussion about using the G12.1 or G112 polar interpolation canned cycle for off-center holes, such as bolt circles.

This thread pertains specifically to C axis lathes that do not have a Y axis.

Regardless of the machine, it is not possible to rotate the C axis 360 degrees while the tool is engaged in a bolt circle hole without cutting through the side of the hole and creating a circular slot on the face of a part.

See the photos above that have 4 holes on the face of the part. Imagine if the tool was inside one of those holes, and the C axis rotated 360 degrees.

Instead the tool must cut small sections of the hole by utilizing the X and C axes simultaneously, until the hole is complete.

The core argument was that it doesn't leave nice finishes, and is a painful procedure with small, deep holes when factoring entry/exit moves and cutter comp initialization.

The code that Rocketmachinist shared sparked a tangent conversation about using Y coordinates on machines that do not have a Y axis.

Apparently Rocketmachinist can enter Y coordinates inside of the G112 canned cycle without getting any alarms, even though his machine has no Y axis.

I was unaware that a machine without a Y axis could do this.

Each machine is different and I have done this very you are trying to accomplish many times over the past 30 years. Not sure what the big deal is telling us what machine you are running this on. Yes it is a pain why most people will use 3 tools on small holes. A Spot or Center Drill, Drill and then Reamer for tight tolerance small holes and not try interpolate it. Not sure what to tell you since you have been forced to go about it this way then you will have to deal with the issues it presents.

Yes Rockertmachinist can do that on a HAAS again why I am asking the machine. A HAAS, MORI, MAZAK, NAKAMURA TOME, OKUMA, HWACHEON, Hartdinge and other machines all do it differently and as much as you think one size fits all it doesn't. 

I will ask the question again in bigger letters since you have missed it 2 times previous.

Have you check the center line of the live tool to the center line of the machine? Yes or No?

Link to comment
Share on other sites
25 minutes ago, mayu said:

Yes they are on-center.

Thank you.

Have you had the machine tuned for this type of work at those speeds and feeds? People don't realize that machines need things tuned in sometimes when doing Multi axis work. At the speeds and feeds you are trying to accomplish this task you could have a mismatch on the servos with a imbalance of weight to spin ratios. When this happened we sometimes will hear a machine humming or will see inconsistent movements when doing work as you are trying to do. Not as noticeable when taking long nice sweeping moves, but in small features where the machine cannot adjust the moves correctly then we see this more. Certain model machines are known for this, but since you refuse to share the make and model of the machine then I can not tell you what to check for and where to check on the machine. Get a hold of your service people and ask them if they know of the parameters you can adjust to tune in the C axis to the X Axis. Other thing could be bad bearings on the spindle because it is old and tried or has been beaten up. Many things to explain why you are seeing what you are seeing, but you are fixated on this Y and C issue and not looking to other factors that could be the issue here. Again why I asked about the machine since I have done this for over 30 years and been around about every brand out there. I know certain things and try to be very careful to not to throw brand under the bus so to speak, but even the best brand if not treated correctly will not do a good job.

I was doing a micron tolerance job on a Mill/Turn and it was coming out awesome. They asked me to rough some huge rings on the machine. I throw these 24" Rings on the machine and started going to town roughing them. That job lasted about a month and then they set the micron tolerance job back up and it was terrible. They scream at me about bad code and 10 others thing I had done in the program. I called the service folks up and had them give me the parameters to check for the turning since we had been pushing the machine so hard I suspected something went out of tune. I spent about an hour tuning the C axis back and and the job like was originally done ran great. They then realized if they wanted to so heavy duty roughing and tight tolerance work on the same machine that was not going to work. They made one machine the roughing and not as tight of tolerance work and the other machine the light roughing and tight tolerance work and life was good. The roughing machine has to be tuned every 6 months the light roughing machine every 2 years.

Sometimes there more going on to the equation than just code and I am trying to get you to think outside of the box so to speak and explore all possible methods and ways that could be creating the issue you are seeing. Please see I am trying to help educate you and not dig on you.

Link to comment
Share on other sites

Thank you for your time and for sharing that - I don't take it personal - interesting story.

I edited the reply above - It's a Samsung with an Oi-TF control. I posted a code snip too.

You're right I'm fixated on the code and the Y C issue - probably because the boss claims this was supposed to be a 20 minute setup, and that the machine is perfect - those are his most common phrases.

Time to call the technician.

Another thing strange is that when polar is used to bore out ID holes, they are consistently .01" small.

We'll see what the tech says.

Link to comment
Share on other sites
47 minutes ago, mayu said:

Thank you for your time and for sharing that - I don't take it personal - interesting story.

I edited the reply above - It's a Samsung with an Oi-TF control. I posted a code snip too.

You're right I'm fixated on the code and the Y C issue - probably because the boss claims this was supposed to be a 20 minute setup, and that the machine is perfect - those are his most common phrases.

Time to call the technician.

Another thing strange is that when polar is used to bore out ID holes, they are consistently .01" small.

We'll see what the tech says.

Code looks correct from they sent. That is just an arc called out to swing a 360 in one line verses being broken up in quadrants. 

Need to get them to come show you how great it is doing that same cut and holding a tight tolerance. If you have Capto or other quick changes tooling and a Hainbuch or Royal Quick change called then yes might be a 20 minute setup, but proving out code is not part of the setup. If the machine and other things are fighting you then it can take all day proving out the code and perfecting the process, but that is not in reality setup time that is prove out time.

Link to comment
Share on other sites

You could test the code they sent by doing shift to move it off X0 to maybe X3.0 and see how it runs on the machine. Would just be like so. Then test out at 6" and see if the machine handles its. If not that supports the machine is not working as expected and needs to be looked at. Brand New machines still can cut bad parts now sure how many time I have had to prove, but I quit counting.
 

G0 X3.0 C0
G12.1
G1Z-.1F10.
G3X3.5I.125C0
I-.25
X3.0I-.125C0
G1Z.1
G13.1

 

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...