Bridgeport gx-480 with fanuc oi-MD control

[Metalurgent]

Two days ago I started a job.
The previous guy is gone, there are no manuals and I'm pecking around the internet and youtube trying to figure this machine out. This is my first time with a Fanuc control after Haas and homebrew CNC UI's. They want parts made, I'm freaking out.
The machine came with a renishaw probe and toolsetter, with macros scrawled on the machine to send into MDI. The macros do their thing, but the offsets are not updated to the machine. I want to disable the probes etc and get back to basics.
I can change tools,
I want a bare-bones approach to setting tool offsets and work offsets.
I followed a number of videos and I'm making some progress
Set gage height of spindle nose to fixed height off table ( in my case 6.375", block plus gage pin), Reset origin, done.
If I load up say, tool 6, T6M06, I can measure and load the offset into the tool table with the INP.C key.

Question (1) For a bare bones setup, I put the offset into offset H001. Will the post default to offset H1 in a program? I have some simple test programs ready to run, but the FUSION360 post doesn't have any G43 callout that I can see to pick the height offset. The suggested post was "generic fanuc"

Question (2) When I change to a new tool and input a new height offset in the screen, the offset doesn't get saved. I see the current tool number displayed on the screen, I can update the number, but when I cycle the tools and come back to that tool, the offset is still set to the offset of the last tool measured.
**Because this machine was set up with probes, Is there a setting that I need to change to allow me to manually change offset?**
Is it possible that I'm missing some process to highlight the current tool so that the control "sees" the offset? I'm just entering the value in H1, with Z- INP,C.

When I display the tool offsets page , it looks the same whatever tool is loaded but with the current tool number at the right bottom of the screen.

My guess is that I could set up the machine with one tool , one tool height offset, one work offset and run something. But I need to run multiple tools and setting the offsets is driving me crazy. I know the Fanuc front end is apparently quirky. It's probably something simple. I've watched lots of videos, went all over the web. I'm stuck and I need the paycheck. If there's anyone out there game to talk me through it , I would appreciate it.

Steam coming out my ears.

 

[Metalurgent]

In a related note, Is there a screen on the fanuc that shows a list of current tools with the associated offsets, tools 1-20 ? There was on the Haas control and it was handy to compare offsets to spot oddball mistakes..

 

[Metalurgent]

Maybe the format is that the offset for T6 would typically be input into H6?

 

[13engines]

The machine came with a renishaw probe and toolsetter, with macros scrawled on the machine to send into MDI. The macros do their thing, but the offsets are not updated to the machine.

With the trouble being had with offsets... are you sure about that?

Your offset number for T6 can be any offset you want it to be, as long as the relationship is carried through when G43 comes around. Though it's certainly common practice to assign the same offset number to the tool number. Keeps things easy.

Until the machine sees G43 with a different H number, or the existing offset is canceled with G49, it will retain the previous amount until it is told something new. Meaning G43 with another H number. What's currently on the screen doesn't matter. How the tool behaves and what your Distance To Go says on the Check Screen as the tool approaches the work is what matters. The display of Current Tool and active G, M, and H codes will change as they are told to. Meaning putting tool 6 in the spindle does not automatically update the current Tool Offset until again... it see G43 with a new H number.

 

[13engines]

Hey metalurgent... I'm not sure my post gave you any help. Was kinda in a hurry and didn't answer your questions directly. I know Fanuc but not familiar with the Oi MD control. Can you take a picture of the Tool Offset Geometry screen, and a picture of your setup with tool measuring device and a piece of raw stock mounted? Also maybe a copy of what your tool setter command line looks like. Could likely help better. Seems like you're working a Tool Setting system where you're not measuring directly on the part, but on a setup device or block on the table. Are you typically setting any numbers in your Work Offset Z settings or are they kept at Zero? Using your setting device on the table leads me to believe you have Z entries in all of your Work Offsets. Not a bad thing, just a thing to know.

I also went on youtube looking for Oi-M Offset Setting help. I found nothing but poorly done time wasting garbage. No wonder you're still having trouble.

 

[Metalurgent]

Thank you very much for the offer of help. I left the job earlier today before I saw your post and will be back again on Wednesday morning. I'll follow up with some screenshots then.
I went back to messing with the probing system. The setter and probe were apparently fitted at the factory and appear to be doing something. I zeroed out the offsets, did a probing sequence and the numbers changed in the tables. I'm probably missing some information on what to add or subtract from the probed numbers to make the work offsets accurate/
I'd like to just get one tool working as a sample, set its height, use it as a master tool to find a G54 X0,Y0, Z.
Then to check things, assuming say T6,
run G54 T6M06 G43H6
G1 X0 Y0 Z1 F50
in MDI and have it do something sensible.

I'd really prefer to do all the setting with an indicator/master tool off a block on the table just so that I'm in familiar territory and not depending on the Renishaw. I'm sure its an awesome piece of kit, but its another level of complexity between me and what's going on.
Trying to get this worked out from internet videos is really difficult.
Lots of video makers zip through stuff like they're on stage performing magic tricks, the object seemingly to bamboozle the audience and have them clap anyway. I get it, though. Teaching and training isn't easy and a lot of these guys are just showing what they know with no intention of being professors for frustrated "In-at-the deep-end, First day, Control Newbies".
I saw a couple of videos where there was a measured effort to convey the information and those were really handy. I'm used to just having the manual and hacking away at it bit-by-bit or having someone show me the basics on day one. Its not like a video game where you can crash and die a hundred times while getting towards your high score.
One crash on this thing before I've even produced a single part and I'll be looking for another arcade.
I'm sure there is a link somewhere to a programming manual for this machine and the oi-MD control
The boss has suggested that he would contact Bridgeport to get one, but I'd really like to find something relevant that I can study before I show up again on Wednesday and spend another bunch of hours tapping on control buttons without chips coming off.

Thanks again,
Metalurgent.

 

[BALNH]

Just a heads up, Z input C inputs relative position.
To set a tool length- touch your spindle face to your 6.375 block. Go to your position screen and origin the Z relative (just type Z and origin should pop up on soft key) Now in MDI change to the tool to be measured. Touch that tool to your block. Go to your offset geometry page, highlight the h value you want to measure ( tool in spindle) and press Z Input C soft key. This will be a positive value. All tools will be different depending on stick out. Do this for all tools to be measured.

You can set the G54Z with any tool you just set/measured. For example T1 measured 4.502. Call tool 1 into spindle and touch off top of your part. Go to work offset screen, under G54 offset highlight the Z. Type Z4.502 then the measure softkey. That will set your G54Z part zero. This will be the machine position distance from home position to your work piece Z0.
Post your NC code so we can what fusion is outputting.
HTH.

 

[Metalurgent]

Hi,
I found this guy on the tube to be very clear, and this was the procedure that I was following.

.
BALHN confirmed that system, but I was still having trouble.
Operating from memory...and studying the video at home, I can maybe see the issue?

I would follow the setup instructions setting the origin ( which I'm assuming is just a Z setting?)
I would touch off the tools and enter them into the offset page.
The first mistake I was making was assuming the offset page was unique to each tool. It's apparently just a list of available offsets to be called within the program. This differs from my older mills where the offset was linked to the tool and called automatically.
So, I look closer at the Fusion post and I see that, by default, it calls out an offset with the same number as the tool. So I enter my offsets in the matching H number, Tool 6 offset in H6.

This makes more sense when I see there are 20 pockets in the carousel and the tool offset page that I inherited has about 20 offsets listed.

I load TOOL6 in MDI.....................................T6M06.
I move to the work offsets page, and use the current tool to set up the G54 offsets.
Move the tool to the desired X0, Y0.
Move the tool down to the desired Z0, PRESS Z [H6 value] MEASURE.
Press [RESET] to check that the Z value updates in the RELATIVE POSITION DISPLAY.

Highlight the G54 X line..
Input [X0] Press MEASURE soft key.
Press [RESET] to check that the X value updates in the RELATIVE POSITION DISPLAY.


Highlight the G54 Y line..
Input [Y0] Press MEASURE soft key.
Press [RESET] to check that the Y value updates in the RELATIVE POSITION DISPLAY.

So then I wanted to check if everything is set up properly.

I go to MDI, and Here's where I think I'm screwing up...

G54 G1. X1 Y1. F25.;
G43 Z1. H6;

When I hit cycle start, the Z seemed to be close but the X and Y headed to the hills.

I think I left out the G90 in my test lines. Does that make sense?

It should read:-

G90 G54 G1 X1. Y1. F25.
G43 Z1. H6.

I added the G90 in MDI after closely looking at the linked video.
I'm not going to be at the machine until Wednesday. Does not having the G90 in place cause the machine to default to a previous offset ( maybe one used by the probe..) and give me the slow runaway to maybe the machine 0?

It would be cool if its that simple.

I've added what the fusion post is giving me for a simple contour with T8.
Looks like there is a default to offset H8 for T8.
I didn't spot that initially. Too much all at once.
Does anything jump out from this program that I should watch out for??

Again, thanks for for taking the time to respond.

Metalurgent.

O1001
(T8 D=0.375 CR=0. - ZMIN=-0.438 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR1)
N30 T8 M06
N35 S9000 M03
N40 G54
N45 M08
N50 G00 X6.3125 Y-2.9625
N55 G43 Z0.6 H08
N60 G00 Z0.2
N65 G01 Z0.1 F42.1
N70 Z-0.2125
N75 G18 N290 G01 X6.2375
N295 G18 G02 X6.275 Z-0.4005 K0.0375
N300 G00 Z0.6
N305 G17
=
=

N310 M09
N315 G28 G91 Z0.
N320 G90
N325 G49
N330 G28 G91 X0. Y0.
N335 G90
N340 M30
%

 

[BALNH]

Hi,
I found this guy on the tube to be very clear, and this was the procedure that I was following.

.
BALHN confirmed that system, but I was still having trouble.
Operating from memory...and studying the video at home, I can maybe see the issue?

I would follow the setup instructions setting the origin ( which I'm assuming is just a Z setting?)
I would touch off the tools and enter them into the offset page.
The first mistake I was making was assuming the offset page was unique to each tool. It's apparently just a list of available offsets to be called within the program. This differs from my older mills where the offset was linked to the tool and called automatically.
So, I look closer at the Fusion post and I see that, by default, it calls out an offset with the same number as the tool. So I enter my offsets in the matching H number, Tool 6 offset in H6.

This makes more sense when I see there are 20 pockets in the carousel and the tool offset page that I inherited has about 20 offsets listed.

I load TOOL6 in MDI.....................................T6M06.
I move to the work offsets page, and use the current tool to set up the G54 offsets.
Move the tool to the desired X0, Y0.
Move the tool down to the desired Z0, PRESS Z [H6 value] MEASURE.
Press [RESET] to check that the Z value updates in the RELATIVE POSITION DISPLAY.

Highlight the G54 X line..
Input [X0] Press MEASURE soft key.
Press [RESET] to check that the X value updates in the RELATIVE POSITION DISPLAY.


Highlight the G54 Y line..
Input [Y0] Press MEASURE soft key.
Press [RESET] to check that the Y value updates in the RELATIVE POSITION DISPLAY.

So then I wanted to check if everything is set up properly.

I go to MDI, and Here's where I think I'm screwing up...

G54 G1. X1 Y1. F25.;
G43 Z1. H6;

When I hit cycle start, the Z seemed to be close but the X and Y headed to the hills.

I think I left out the G90 in my test lines. Does that make sense?

It should read:-

G90 G54 G1 X1. Y1. F25.
G43 Z1. H6.

I added the G90 in MDI after closely looking at the linked video.
I'm not going to be at the machine until Wednesday. Does not having the G90 in place cause the machine to default to a previous offset ( maybe one used by the probe..) and give me the slow runaway to maybe the machine 0?

It would be cool if its that simple.

I've added what the fusion post is giving me for a simple contour with T8.
Looks like there is a default to offset H8 for T8.
I didn't spot that initially. Too much all at once.
Does anything jump out from this program that I should watch out for??

Again, thanks for for taking the time to respond.

Metalurgent.

O1001
(T8 D=0.375 CR=0. - ZMIN=-0.438 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G20
N20 G28 G91 Z0.
N25 G90

(2D CONTOUR1)
N30 T8 M06
N35 S9000 M03
N40 G54
N45 M08
N50 G00 X6.3125 Y-2.9625
N55 G43 Z0.6 H08
N60 G00 Z0.2
N65 G01 Z0.1 F42.1
N70 Z-0.2125
N75 G18 N290 G01 X6.2375
N295 G18 G02 X6.275 Z-0.4005 K0.0375
N300 G00 Z0.6
N305 G17
=
=

N310 M09
N315 G28 G91 Z0.
N320 G90
N325 G49
N330 G28 G91 X0. Y0.
N335 G90
N340 M30
%

The relative screen does not update. That screen is more a less a readout to help with setting up. Similar to the operator position page on a Haas. The absolute position page updates after hitting reset, if that offset is active.

In your MDI program section the G1 has decimal but yea the xy should position 1. Inch from your origin. I prefer my positioning in programs to look like this:
G0G90G17G54X_Y_.
Also your NC code is posting arc movements in the XZ plane (G18).

As far as checking tool offsets you can just use a 6in scale with tool in the spindle. Measure from spindle face to tool top to get an approximate length.

HTH