kkominiarek

VMC's with a Fanuc Series 18i-mb control

Recommended Posts

The below section of code backplots and verifies fine.

Operation is standard pocketing with islands using a 3/16 bull mill.

 

 

G1 X2.5182 Y-.4059

X2.8628 Y-.0609

X2.7946 Y-.0142

X2.5833 Y-.2255

G3 X2.6694 Y-.074 I-1.3003 J.8397

X2.6837 Y-.0122 I-.126 J.0618

X2.6838 Y-.0098 I-.1403 J0. (trouble line for johnsford vmc)

G1 X2.7078 Y.0143

X2.816 Y-.0291

 

 

On the Agma VMC the code machines as it should.

 

On the Johnsford VMC the line of code "where labeled" machines a ccw 360 deg circle (dig into island) then continues on the correct path.

 

We had this machine for 4-5 years w/o any issues like this in the past.

 

Both machines have the same control....would anyone know what the issue could be? (a parameter?)

Share this post


Link to post
Share on other sites

The machine doesn't like the .0001" move in X. Change the parameter that breaks the arcs into quadrants so it doesn't break arcs. I had an older machine at another shop I worked in that had problems with that. Hope that helps.

Share this post


Link to post
Share on other sites

Goto settings

config

tolerances........ Whats your min. arc length set to?

Share this post


Link to post
Share on other sites
G1 X2.5182 Y-.4059

X2.8628 Y-.0609

X2.7946 Y-.0142

X2.5833 Y-.2255

G3 X2.6694 Y-.074 I-1.3003 J.8397

X2.6837 Y-.0122 I-.126 J.0618

X2.6838 Y-.0098 I-.1403 J0. (trouble line for johnsford vmc) (shouldn't the X be the same or smaller number [depending on rounding] than the previous X)

G1 X2.7078 Y.0143

X2.816 Y-.0291

 

 

I'm thinking the Johnsford is correct and the Agma is misreading.

Share this post


Link to post
Share on other sites

The below section of code backplots and verifies fine.

Operation is standard pocketing with islands using a 3/16 bull mill.

 

 

G1 X2.5182 Y-.4059

X2.8628 Y-.0609

X2.7946 Y-.0142

X2.5833 Y-.2255

G3 X2.6694 Y-.074 I-1.3003 J.8397

X2.6837 Y-.0122 I-.126 J.0618

X2.6838 Y-.0098 I-.1403 J0. (trouble line for johnsford vmc)

G1 X2.7078 Y.0143

X2.816 Y-.0291

 

 

On the Agma VMC the code machines as it should.

 

On the Johnsford VMC the line of code "where labeled" machines a ccw 360 deg circle (dig into island) then continues on the correct path.

 

We had this machine for 4-5 years w/o any issues like this in the past.

 

Both machines have the same control....would anyone know what the issue could be? (a parameter?)

 

Hi!,

 

If you got the answer for this problem ??

 

Please let me know .

 

Thanking you.

 

regards

Nitin

Share this post


Link to post
Share on other sites
Guest MTB Technical Services

The Parameters for processing Arcs are most likely not the same on both machines.

 

 

The easiest fix is to simply change you control settings in Mastercam to

 

1) Change the minimum arc distance and break arcs at 180 increments.

 

or

 

2) Change the output to use R-Words arcs instead of I & J.

Share this post


Link to post
Share on other sites

The Parameters for processing Arcs are most likely not the same on both machines.

 

 

The easiest fix is to simply change you control settings in Mastercam to

 

1) Change the minimum arc distance and break arcs at 180 increments.

 

or

 

2) Change the output to use R-Words arcs instead of I & J.

 

Hi!,

 

Thanks .

 

I changed the control setting :

 

Minimum arc radius = 0.02

 

& break arcs at quodrants .

 

You can see the line where arc is taking longer path than a shortest path. Only when there is a small diffrence in X or y postion in circular path

 

 

N5188 G2 X-30.783 Y137.992 I22.175 J-90.224

N5190 G3 X-26.7 Y136.305 I4.083 J4.096

N5192 X-26.661 Y136.304 I0. J5.783

N5194 X-25.882 Y136.378 I-.172 J5.922

 

I do have few queries :

  1. why do we need minimum radius as : 0.005 or evn 0.1 when we knwo that we cannot machine lower than cutter radius

  2. In some case default max radius is given 200 mm : It should be maximum so as to allow lrger arcs i. 9999mm or more

  3. Tolarance in surface toolpath where this error is geneating i.e Surface finish contour : 0.001 is default value : we changed later to 0.01

  4. What is the setting required in machine controller . Any machine parameter ?

  5. Problem is due to machine taking larger portion of arc at this location see image attached.

Thanking you for your suggestions !

 

regards

post-12508-0-23840400-1371471673_thumb.jpg

Share this post


Link to post
Share on other sites

N5190 G3 X-26.7 Y136.305 I4.083 J4.096

N5192 X-26.661 Y136.304 I0. J5.783

 

verry small change in Y as above is causing the problem ?

 

Would you please modify MasterCAM of output format?

Or, you may try parameter N5008#5 from 0 to 1 to check any improvement.

 

 

N05008 P 00
0
00000
à
P 00
1
00000

 

This is because Fanuc controller has calculated the command of path.

However, the two points are too closed for G02/G03 moving which is like a straight line.

Fanuc will think to run path with big arc.

Please refer it.

 

OTHER REF.: see some solutions provided by machine tool supplier

post-12508-0-18921100-1371472922_thumb.jpg

Share this post


Link to post
Share on other sites

we had a simmeler problum with two parts in a row, never had a problum with the machine befor, master cam was not caculating the right end point or swing point of the arc the progamer drew it out on the computer and it was not the right numbers, the machine should have alarmed out, but the parm was set big enough to let it keep going, the only thing that fixed it was to set to the no rounding setting we reran prog meny times with diffrent settings, but no rounding was the only fix for us

Share this post


Link to post
Share on other sites

We tried a few things....nothing worked for this particular issue.

 

Our vendor had us change parameter 3450 and 5008......this did not work

Add lines...G49 G40: G5.1 Q1: before the G43 H4 Z.3:.....this did not work

We tried the parameter change with and without the G49 G40: G5.1 Q1:....this did not work.

 

We had no problems before and no problems since.

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