medaq

Fanuc d offset help

Recommended Posts

Hey everyone,

 

God need to fix a annoying problem.

 

We have a annoying problem on our fanucs, And with us removing alot of the non fanuc machines out the door. For the new fanuc coming in. The guys who are used to fadals and the yasnac i-80 are going to scrap some parts.

 

Here is the problem, Now I have known about it, on our es 450's but since I only program them I never worried to much about it.

 

But this morning retroing a fadal chamber program to the chevalier fanuc o-m I almost scrapped the part.

 

The problem is fanuc does not have a seperate offset section for d offsets. The fadals have em and the enshu has them. But our fanucs dont. Which I find kinda retarded.

 

So I am contouring a small whole, Reading the numbers on the screen. When I go to do the contour where it should have a .1 perpendicular entry, The screen reads something like 11.5"s to go.

 

What happens if you forget to change the d offset to some number that is not a height offset then it will try to pull off a 11.5" comp. I wish it would alarm out when the vector is shorter than the offset being called. it does this on fadals and the enshu.

 

Now with a machine coming in with 240 tools. I see this being a problem for me and the other programmer. If you have a wrong comp, the spindle could try and comp its way right into your pallet. I have seen this on the es450's. Always scares the crap out of me.

 

So is there a way to force the post to increment the offsets a set amount. No matter what is in your tool operations page?

 

Meaning if I make the force 20 tools. T1 will always have t21 no matter what. Or 240 tools will have d 241 for t1 no matter what.

 

I no in the job setup page you can type in the increment amount. But this does not help when grabbing old programs to fit onto the new controls. You have to go to each tool operation and change it. some of our programs have 200 operations. Making it very time consuming.

 

So is there a way to force this in the post?

 

Jim

Share this post


Link to post
Share on other sites

Well to be honest the best thing I can tell you is to use wear on a Fanuc. Get your guys use to Zeroing out the offsets every time they change a job and all will be good. If it is a 240 tool then I would go T1 D251 and go from there all of your D's can be changed thru a post for posting or you can change it on the tool parameter page. Some of the newer Fanucs do have a separate page for Diameter offsets.

 

HTH

Share this post


Link to post
Share on other sites

It is not about zeroing out the offsets. It is about g41 d1 and using -12.5" as a offset.

 

I was just curious if there was a way to force the post to do the add in the of the offsets. Instead of it ever accidentaly using d1 as a offset. It would automaticaly use d251 as a offset and so on and so on.

 

Jim

Share this post


Link to post
Share on other sites

Good Day ,

 

What Crazy says is if you output:

G43 Z# H1

G1 Z-#

G41 X# D1

 

If the length (H) is 12.5 then the (D1) will

also read the 12.5. If your machine has 30 tool

magazine, then the first D# for tool 1 is D31.

 

Fadel and Haas and yasnac can use H1 and D1.

 

HTH

 

Tony G

CNCiT Precision Machine - Hudson,NH

X Beta Site

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

 

MasterCam X "Has made my job a "Hole" lot easier"

Share this post


Link to post
Share on other sites

Good Day ,

 

If you go to job setup, you can set the tool offset registers for length and diameter to add

an amount to give you H1 and D31.

 

Using this feature will only work on a new mastercam session, not an existing file.

 

This can also set in screen -config. -NC settings

-Operational defaults

 

Tony G

CNCiT Precision Machine - Hudson,NH

X Beta Site

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

 

MasterCam X "Has made my job a "Hole" lot easier"

Share this post


Link to post
Share on other sites

quote:

Using this feature will only work on a new mastercam session, not an existing file.


I understand the h1 -12.5 is d1 -12.5. What I am hoping is a hard fix to my post. To force that d1 to be d31 permanetly. So the programmer myself has no choice for a different d offset. I dont see any use to ever have multiple d offsets to my tool. And if I need it I can hand edit the one I need. I rather have safety of parts than anything.

 

 

All I am asking, is there a way to hard code it into the post to permanetly add the 30+ tool offsets or 250+ with the nig changer. So every time I use the post for the specific machine I dont have to worry about going through 200 tool operations making sure of the d number is already added in.

 

So g41 offset would have something like this in the post. I am sure there has to be a way. But I am not post savy enough to know exactly how. I dont even want the post to get the information from the tool page. I just want it to do it no matter what.

 

d = t + 30

Share this post


Link to post
Share on other sites
Guest CNC Apps Guy 1

code:

pccdia2    # Cutter Compensation

tloffno=t+30

if ccomp <> 4, tloffno

This works for me...

 

HTH

Share this post


Link to post
Share on other sites

Thanks james this is what I am looking for. Only problem for me I do not see pccdia2 in my posts.

 

I have this

 

pccdia #Cutter Compensation

#Force Dxx#

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k

sccomp

if cc_pos, tloffno

 

 

What would you do to this to make it work? chop it out and write what you wrote?

 

Jim

Share this post


Link to post
Share on other sites

James

Would it be

 

if cc_pos, tloffno + 30

 

or does he need to look search for 'tloffno' somewhere else in his post

Share this post


Link to post
Share on other sites

You need tool offset c so you can use one offset for both D and H

 

ie G41D1Y1.

G43H1z1.

 

this is an option from fanuc

rgds

George

Share this post


Link to post
Share on other sites

medaq,

If you're getting a 240 tool machine, just pay the $4,000 or so and get the diameter option. Then you can have H1,D1.

Share this post


Link to post
Share on other sites

Find tloffno in Format section:

fmt D 4 tloffno

change to:

fmt D3 4 tloffno

 

This will force D31 on T1 on older programs that you have, if you change job set-up to add 30 later..this fix will be a mess.

Share this post


Link to post
Share on other sites

quote:

If you're getting a 240 tool machine, just pay the $4,000 or so and get the diameter option. Then you can have H1,D1.

If I knew it was a option, I would of purchased it in a heart beat. Maybe it is going to come with it, atm I dont know. But I would still like to solve this problem on my 2 es 450's and the fanuc o-m control we have.

 

We are getting the matsuura, It comes with something called handyman2? I have never used it.

 

Jim

Share this post


Link to post
Share on other sites

It can also be done from job setup in mastercam

in job setup on the right tool registers chose add to and put in what you want it start at.

Share this post


Link to post
Share on other sites

medaq,

Change your post to:

 

#######################################

pccdia #Cutter Compensation

#Force Dxx#

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k

sccomp

tloffno = tloffno + 20

if cc_pos, tloffno

 

###############################

The post is the correct place to take care of this.

Share this post


Link to post
Share on other sites

Hey brian just changed what ytou recomended on a test post.

 

It works and doesnt work at the same time smile.gif

 

The g41 line worked just like it should of.

 

d1 became d21

 

But every other line added in d+20

 

So the next line had d41 the d61 and so on till g0z.1 then started over at d21

 

Jim

Share this post


Link to post
Share on other sites

Medaq.

Put tloffno=tloffno+xxx where xxx is the number you want to add to the offset, at the begining of post blocks, psof, ptlchg, and ptlchg0.

The reason you put it in psof is for the start of the program i.e. the first tool. And it is obvious why you put it in ptlchg. The reason you put it in ptlchg0 is, for some reason you want to use two dia offsets for the same tool, you can do that also. HTH

 

Rob

Share this post


Link to post
Share on other sites

Well the good news, we called up the manufacturer of the machine. And they just gave us the bit number to turn the d offsets on. And with the new matsuura install. I am sure they will turn it on the es450's we already have if I ask nicely and give him a 6 pack smile.gif

 

Jim

Share this post


Link to post
Share on other sites

Not to hijack your thread medaq, but... I have the d offset on my Fanuc 16. The one thing I have never played with is the wear functions. What do they do? Looked around the manual but you know how helpful those are. Just wondering.

Share this post


Link to post
Share on other sites

ghuns,

Are you referring to the wear offset on your control?

If it's the same as my 10m/11m its just a fine tune offset.

If you wanted to keep the original offset there,you can change the dia by putting a value in the wear column.

HTH

Share this post


Link to post
Share on other sites

Yep, the one in the control. So it just adds to the # in the H or D row. I get it. Learn somethin new every day.

Share this post


Link to post
Share on other sites

My bad.

 

change "tloffno = tloffno + 20"

 

to "tloffno = t + 20"

 

that will correct the problem where D continues to increment by 20.

Share this post


Link to post
Share on other sites

In the post directory of the FTP, these is a post Mill_Haas_VF

 

This post includes the following options, and is a good example for automating the tool offsets.

 

h_offset : 0 # Length offset method

# 0 = H value is always same as Tool number

# 1 = H value as set in Mastercam tool parameter (from NCI file)

 

d_offset : 0 # 0 = D value is always same as Tool number

# 1 = D value as set in Mastercam tool parameter (from NCI file)

# > 1 = D value is Tool number plus value of d_offset variable

Share this post


Link to post
Share on other sites

great thread i have a old fanuc . been dealing with same problem. james that bit of code worked perfect. i,m glad i ran across this.

 

 

have a good day heavy

Share this post


Link to post
Share on other sites

Sorry to dig up an old thread but this is almost the exact situation at my current shop I am dealing with. we have 3 of the exact same model and control ES450's in our shop. 2 of them have the "type C' offset table that has 4 columns (H, H wear, D, and D wear) The last machine has the "type B" offset table with only 1 column of just basic offsets numbered 1-99

I have the same issue where if I give a program to a setup guy and he sets it up on the type B ES450 without altering all of his programmed D values, the machine will crash when it called up the tool length as its D offset and tries to make a -10" offset 😑

Does anyone know if the upgrade from type B to type C offset tables is something that can be done in house with a parameter change? Or do we need to get with FANUC??

All 3 machines are 1997-1998 Matsuura ES-450H models with Fanuc 18i-M controls which is why I was hoping it was a simple parameter change.

 

thanks for any help or direction

fanuc type B offset table.jpg

fanuc type C offset table.jpg

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