Hartford HV-35 tool change and Z-home problems

Hello.
We bought Hartford HV-35 with Fanuc OMC, year 1993. This is my first cnc mill. Boss bought it for me to learn cnc programming and for milling plastic parts. At the beginning I had few problems due to my lack of knowledge and experience, but once I got it to run I had no problems.

Mill was not in use for some time. Then I started milling parts again and sometimes mill wouldn't finish tool change. Spindle goes in place for tool change, umbrella goes out and grabs tool. Then sits there until error "not fin". Then I turn machine on and off to release air pressure in cylinder that moves umbrella tool holder back. G28 x0 y0 z0 and manually change tools few times or start a program. Programs are short, less then 5 min.
After a while I started paying attention to what could cause this errors. My first thought was that machine Z0 is too low and umbrella is forced down quite a bit at tool change, and tool pockets show a lot of wear. So I tried moving metal trapezoid that triggers a switch at home position. I move that for about 10mm up, and machine measuring system moved only few mm up. I also tried cleaning the switch, didn't have much effect. Greasing tool holders seem to help.

After that I noticed glitches on Z axis 3 times. First time I was using tools 2, 3. Tool 2 didn't go low enough. It was programmed to go for example z-10,0 and it went only 9,7mm. I corrected to -10,3 and it still went only 9,7mm down. Machine red as -10,3 but calipers measured 9,7. I took 20mm gauge block and machine red z0,3. Corrected that to z0 AGAIN and started a program. Again same problem. Then I turned machine off for few minutes and back on. use g28 for home position, Z was wrong jet again. At that time I left it like that because parts were finished from the other side and depth of this hole was not important as long as diameter was OK.

Same problem, different part. I thought it was my fault.

Yesterday I was milling plastics, program was already written and tested. I was using tool 2 and 3. I put clamping stencil inside a vice. Took my zeros with dial indicator and Z with 20mm gauge block. Wrote down machine coordinates. First part was ok, second was 0,8mm too low. I made few bad parts...
I took a look at machine coordinates written on paper and in G45, G55 they matched! It is in possible that I would write 4 digits wrong. Then I took gauge block and touch it with mill, machine coordinate was 0,8 lower then at the beginning!

-Does machine check (and re writes) it's Z0 every time that it preforms a tool change? If so, then Z axis home position switch is bad.

-If I start a program that has M6 T2 at the beginning and T2 is already in the spindle, Z would go down ( probably to its lowest possible position), then up to machine Z0 and then start milling. At this point start/stop buttons will not stop the movement, only reset will. After this action is performed I can just hit stop button and machine will stop moving but spindle will still turn. So if I use multiple tools I always have to preform tool change at the beginning of a program, or use a single tool and not specifying which tool it is. Fanuc lathe doesn't have this problem. What could cause this to happen?

Any help will be appropriated!

Have you taken the z-axis home switch apart and cleaned it?
Sometimes the buttons that press down the microswitches inside get stuck or dont move free enough.

kemenb said:

-Does machine check (and re writes) it's Z0 every time that it preforms a tool change? If so, then Z axis home position switch is bad.

Click to expand...

The switch its self doesn't set the exact zero position. That's still a specific pulse off the encoder. The switch only indicates your on that turn of the screw. If you noticed, the reference return will semi - rapid until it hits the switch, them slow down, and it will find the reference pulse once it comes off the switch dog But the true position still comes off the encoder. That's as accurate as any other position of the encoder

A switch problem normally happens if the switch is faulty and it over travels, or jumps one pitch of the screw. An error is 0.8mm isn't due to a switch.

Hartfords I've played with use G30 or a second reference position for toolchange positions.

Regards Phil.

There are a couple things that could be wrong. I think starting at the most basic point would be helpful. So how about posting some examples of your code.

A few ideas...

Make sure your Z axis work shift is set to 0.

Rather then rapiding at 100% in Z down to the top of the part, try going slower. Put an indicator on the table and write some code so that the spindle face touches the indicator and zeroes out. Try at different speeds from home and see if it repeats. Maybe the pulse coder is losing count at higher speeds.

What is the max rapid traverse in the Z axis? I'm curious.

Make sure your tools are getting properly seated in the spindle taper.

The crazy unstoppable tool change movement I'd guess is because the tool change command is a macro program. Parameter 10 bit 4 equaling 1 hides these 9000s series programs. If you change the bit to 0 you can see the program. This code is either macro A or macro B. There is another parameter that controls whether single block will stop these types of programs. It might also be the same for feed hold. I'm not sure of that parameter off the top of my head. Maybe the code is written into the ladder of the machine, but it's easy enough to check.

Post some of your code just to make sure there's nothing weird about it and I'm sure some folks will chime in.

That was fast!

@tkgb: I took Z switch of the machine, took it apart, cleaned mechanical components with acetone. Checked switches with multi meter on diode setting that beeps. Before assembling the switch I sprayed with silicon spray. Assembled and checked with multi meter again.

@mattedroom: there is a program called ATC (automatic tool change) in the library, but I can't remember its number. I opened it once out of curiosity. It's G code, with if/else sentences and needs some parameter to even view it.

Most of my programs are for milling holes in two parts at the same time, so I use G54 and G55. Parts are side by side and have different Y. Rapid feed is at 18.000mm/min, but I usually work at 25%. Work feed does not exed 350mm/min. Everything over 300mm/mim will make holes too oval. Spindles have a lot of play in them! Y axes has at least 0,07mm.
I wrote this as an example, I can snap a photo or write the one from yesterday on Monday.

O0095 (PROGRAM NAME);
G90 G54;
M6 T2;
M3 S2000 F250
G0 X-40.0 Y0 Z20.0
Z1.0
M98 P1001

.O1001
.G1 Z-7.6
.G91
.X-3.1
.G2 X6.2 Y0 R3.1
.G2 X-6.2 Y0 r3.1
.X3.1
.Z-6.0 and repeat this process
.G90
.G0 Z20.0
.M99

M6 T3;
M3 S1600 F180
G44 H3
G90 G54
G0 X-13.0 Y0 Z20.0
Z1.0
G1 Z-20.3
G0 Z20.0
G55
G0 X-13.0 Y0
Z1.0
G1 Z-20.3
G0 Z20.0 M5
X180.0 Z200.0
M30

Do as suggested with an indicator pointing up at the spindle. Remove tool. Write a program that moves Z up and down at different speeds. See if it re-zeros every time or if not at what speed does it start having problems. That should tell you if you have encoder problem or homing problem.

kemenb said:

@mattedroom: there is a program called ATC (automatic tool change) in the library, but I can't remember its number. I opened it once out of curiosity. It's G code, with if/else sentences and needs some parameter to even view it.

Click to expand...

Hello kemenb,
Take a look at the following parameters:

Parameter --------- Program Number
0230 ------------------ O9020
0231 ------------------ O9021
0232 ------------------ O9022
0233 ------------------ O9023
0234 ------------------ O9024
0235 ------------------ O9025
0236 ------------------ O9026
0237 ------------------ O9027
0238 ------------------ O9028
0239 ------------------ O9029

0240 ------------------ O9001
0241 ------------------ O9002
0242 ------------------ O9003

Look for the number "6" being registered in any of the above parameters. The Tool Change Macro program will have the program number that corresponds to the parameter where "6" is registered.

If "6" is NOT registered in any of the above parameters, check the value of parameter 0040 bit 5. If set to "1", program number O9000 will be the Tool Change Program.

You will need to set parameter bit 0010.4 to "0" to be able to view and download programs in the O9000 to O9999 range.

Post a copy of the Tool Change Program here for the Forum to see.

I note in your following program that a Tool Length Offset has not been called up for T2 in program number O0095. Then further down where T3 has been called, G44 (Tool length Compensation – direction) has been used. This will work, but its counter intuitive. The Tool Length Offset will be applied in the opposite direction to whatever the sign of the Tool Length Offset in the Offset Registry is.

Regards,

Bill

kemenb said:

O0095 (PROGRAM NAME);
G90 G54;
M6 T2;
M3 S2000 F250
G0 X-40.0 Y0 Z20.0
Z1.0
M98 P1001

.O1001
.G1 Z-7.6
.G91
.X-3.1
.G2 X6.2 Y0 R3.1
.G2 X-6.2 Y0 r3.1
.X3.1
.Z-6.0 and repeat this process
.G90
.G0 Z20.0
.M99

M6 T3;
M3 S1600 F180
G44 H3
G90 G54
G0 X-13.0 Y0 Z20.0
Z1.0
G1 Z-20.3
G0 Z20.0
G55
G0 X-13.0 Y0
Z1.0
G1 Z-20.3
G0 Z20.0 M5
X180.0 Z200.0
M30

Click to expand...

angelw said:

I note in your following program that a Tool Length Offset has not been called up for T2 in program number O0095. Then further down where T3 has been called, G44 (Tool length Compensation – direction) has been used. This will work, but its counter intuitive. The Tool Length Offset will be applied in the opposite direction to whatever the sign of the Tool Length Offset in the Offset

Click to expand...

Writing M6 T2 G44 H2 seemed pointless. If T3 is longer I need to write minus sign in tool offset. There is another way of doing this?

My co-worker told me that he selects master tool (T2 in this case) and applies tool offset for the rest of the tools. He works on old Maho and applying offsets also changes coordinate system, mine does not.

Can you explain this: for example H3=-2.0 (T3 is 2mm longer then T2) and I write:
M6 T3
G44 H3
G0 Z0 machine will go to what I set as zero point. I usually use ALL tab for displaying coordinates so I have 4 sets: relative, absolute, machine, distance to go. Absolute will read Z 2.0 instead of Z 0.0 but it will go to right height. Is there a parameter that will fix that?

Why is relative coordinate system used for?

Tomorrow after work I will try to do what you all suggested and post the results.
Thank you all for helping,

regards Klemen

kemenb said:

Writing M6 T2 G44 H2 seemed pointless. If T3 is longer I need to write minus sign in tool offset. There is another way of doing this?

My co-worker told me that he selects master tool (T2 in this case) and applies tool offset for the rest of the tools. He works on old Maho and applying offsets also changes coordinate system, mine does not.

Can you explain this: for example H3=-2.0 (T3 is 2mm longer then T2) and I write:
M6 T3
G44 H3
G0 Z0 machine will go to what I set as zero point. I usually use ALL tab for displaying coordinates so I have 4 sets: relative, absolute, machine, distance to go. Absolute will read Z 2.0 instead of Z 0.0 but it will go to right height. Is there a parameter that will fix that?

Why is relative coordinate system used for?

Tomorrow after work I will try to do what you all suggested and post the results.
Thank you all for helping,

regards Klemen

Click to expand...

Hello Klemen,
There are quite a few ways to establish Tool Length Offsets. All work, but some are more intuative than others. Some use the Fresh Air gap between the tip of the Cutting Tool and a fixed datum in Z. Other use a Master Setting Tool and calculate an Offset relative to this Master Tool, for all other tools. But overwhelmingly, at least with my clients, the Spindle Nose is the Datum, and the Tool Offset is the length of the Tool from the Gauge Line of the Tool Holder's Taper (corresponds to the end of the Spindle Nose) to the tip of the Cutting Tool. To put it in your terms of Master Tool, the Spindle Nose can be considered as a very short Master Tool, and all other tools are Offset relative to the Master Tool being the Spindle Nose.

One big advantage of using the Spindle as the Master Tool, is that its always able to be found, and it never varies in length.

In your example of T3 being 2mm longer than T2, if you think it through logically, T3 (longer by 2mm) must be moved in a Positive Direction, relative to T2, when it approaches the Workpiece, yet you have a -2.0mm registered as its Offset. By using G44, you're actually reversing the direction of the Offset as its specified in the Tool Offset Registry. Accordingly, the tool that is 2mm longer than the Master Tool and has a -2.0mm Offset will be Offset in a Plus direction when using G44. To me that makes little sense when G43 is available.

Without knowing your procedure for setting Offsets Values, take for example the following manual method of determining a tool Offset.

1. Place Setting Indicator on the table of machine.
2. With T2 (Master Tool) in Spindle, move it to touch off on the Setting Indicator.
3. Zero the Z Relative Position Display.
4. Replace Master Tool with Tool to be measured.
5. Move New Tool to touch off on the Setting Indicator.

If the New Tool is 2.0mm longer than the Master Tool used to set the Z Relative Position Display, then the Z Relative Position Display must now be displaying Z+2.0mm. Would it not be easier to just record the value being displayed (+2.0) than having to remember to change its sign when you register the value? Similarly, if the Tool being measured is 2.0 shorter, when its touched off on the Setting Indicator, the Z Relative Display will be Z-2.0mm and again you would have to remember to reverse the sign rather than merely register the displayed value if you use G44 to apply the Tool Length Offset.

There are many examples when its safer to reiterate code in a program, even when you're sure its not required. At the End of each Tool Operation I have code that will take the Tool to a safe Tool Change position in X and Y, as well as Reference Return position in Z. I repeat this code at the Start of each Tool Operation, so that in the event that I stop the operation mid cycle, I can just place the Cursor at the beginning of the Tool Operation, knowing that the program is safe to start. If I have a program that has 10 Tools, then its made up of 10 Stand Alone programs.

Depending on parameter setting, and the make of the control, Tool Length Offsets aren't necessarily canceled by Reset. Lets take your example of not bothering to specify a Tool Length Offset Call for T2. For some reason there may be call to stop the program mid cycle of another tool where its Length is considerably Shorter than T2 and a Tool Length Offset has been called and is active after you interrupt the cycle. You re-start the program from the T2 operation, where there is no Tool Length Offset called. In this case, if the other Tool's Length Offset is still active, there is a big chance that T2 has just been driven hard into the job. Right about then you may be thinking, it doesn't seemed quite so pointless to specify a Tool Length Offset for T2.

The Relative Coordinate System is very handy for setting up. Its a Position Display that can be arbitrarily set to Origin or to a Specified value, whereas the Absolute System not.

Regards,

Bill

Gratings everyone, sorry I couldn't write sooner.

I touched the dial indicator put X0 Y0 Z0 and wrote some code:
G56 G90
G0 Z0
M00
G28 Z0
M99
At first pass Z stopped 0.01 higher, then I deleted M00, drove Y away so spindle didn't touch dial indicator and left it going up and down for half an hour ant 25%. Repeat this test, then left it for some time at 50% and at the end I even tried at 100%. After machine was warmed up dial indicator showed -0,01. I even tried G0 Z0, tool-change, G0 Z0, tool-change, resultants were in this margin.
Rapid traverse is set at 16000mm/s for all axis, but I never exceed 25% rapid traverse and 350mm/min work feed.

Parameter 230: 00000010 only 9000 series program on the machine is 9020 ATC. I couldn't get it to open this time, even if parameter 10 was 00000000. Checked on the laptop if it is on it, but it is an empty folder. Machine-PC cable works iffy at best (70% transfer success), one direction only. Does any one have a wiring diagram how to make it? I have written all different combinations that didn't really work.

Here is a photo if ATC, it is identical to the one on the machine. I checked it a year ago:


Here are photos of clamp like grippers for automation. We inject mold blank parts from POM and mill out gripper shape. So far I have written about 30 programs and subprograms for various shapes.
When order comes I use hole in the middle of the stencil to get center with dial indicator and write machine values on a paper (at the beginning I wrote them in another separate offset not used by program). Than write machine value in offset, MDI, G54 reset. Go 25,25 in Y+ write machine value in offset, reset. If Y=0 I go to Y-25.52, check if machine value is same as when I found center of the stencil, if it matches I go to Y-51.04, write machine value in offset, MDI, G55 reset, Y=0.
I get X center by touching one of the clamps (top on the photo) and write same number for G54 and G55.
Then I prepare required tools, up to four so far. Clamps are 20mm in height, I touch 20mm gauge block with T2, write machine constant into G54 and G55, reset, check G54 and G55 position. Change tools, touch gauge block. Write - for longer and + for shorter in tool offset tab.
Using G44 and G43 inside my code would probably result in a big mess. I would have to be very careful that each time I'm making same clamp shape I clamp tools in the same height, or check the code every time. 8 and 10 mills can be set in the tool holder so eider one is longer.
If I start using G43 I could just write + for longer tools and - for shorter?



Before tool change Z goes to Z=30mm, M5. When tool change is called and G44 is in use tool first jumps for its offset value up or down and then goes to its home position. Is there a way to skip this part and send it straight to home position?
After tool change I write G54/G55 and G90, so I can start mid program.

Does this Fanuc have block delete or another way to make it skip a line? Didn't find anything in Fanuc manual.

kemenb said:

Parameter 230: 00000010 only 9000 series program on the machine is 9020 ATC. I couldn't get it to open this time, even if parameter 10 was 00000000. Checked on the laptop if it is on it, but it is an empty folder. Machine-PC cable works iffy at best (70% transfer success), one direction only. Does any one have a wiring diagram how to make it? I have written all different combinations that didn't really work.

Click to expand...

Hello kemenb,
If your control is a circa 1980's machine, parameter 230 should be a base-ten integer between 1 and 255 (M98 and M99 excluded), not what appears to be a binary number in your above quote. Look up parameter 230 in the Machine's Fanuc Operators, or Maintenance Manual to see what the purpose of parameter 230. Do the same for parameter 10 is. I'd be interested to know.

If the Tool Change Program being used by the machine is exactly the same as the program shown in your attached pictures, you can't arbitrarily set your control to run a program in Imperial (G20) Mode. The Tool Change Program includes G21 and swapping back and forth between G20/G21 should not be done in a program. One reason being is that Tool Offsets are not necessarily converted.

kemenb said:

Then I prepare required tools, up to four so far. Clamps are 20mm in height, I touch 20mm gauge block with T2, write machine constant into G54 and G55, reset, check G54 and G55 position. Change tools, touch gauge block. Write - for longer and + for shorter in tool offset tab.

Click to expand...

Why write longer tools as Minus and shorter tools as Plus Offsets, whats your logic for doing so? As I stated in my last Post, if you're going to use a Master Tool, simple set the Z Relative Position Display to Zero when you touch off T2 and then just register the Z value as it appears in the Relative Position Display for other tools being set and use G43. And at least use some sort of Master that is not going to change in length. Using a tool that you use for machining will change in length. That being the case, you would then have to set all other tools in the magazine each time there was a slight change in length of T2.

kemenb said:

Using G44 and G43 inside my code would probably result in a big mess. I would have to be very careful that each time I'm making same clamp shape I clamp tools in the same height, or check the code every time. 8 and 10 mills can be set in the tool holder so eider one is longer.

Click to expand...

Why would using G43/G44 in you code result in a big mess. What's going to bite you one day is NOT using G43/G44 to apply the Tool Length Offset of the current tool (see my example in my previous Post).

kemenb said:

If I start using G43 I could just write + for longer tools and - for shorter?

Click to expand...

Yes. If you Zero the Z Relative Position Display when you touch off your Master Tool, you would register the value being displayed in the Z Relative Position Display. If the Spindle Nose is used as the Master, ALL Tool Length Offsets will be Positive Values.

kemenb said:

Before tool change Z goes to Z=30mm, M5. When tool change is called and G44 is in use tool first jumps for its offset value up or down and then goes to its home position. Is there a way to skip this part and send it straight to home position?
After tool change I write G54/G55 and G90, so I can start mid program.

Does this Fanuc have block delete or another way to make it skip a line? Didn't find anything in Fanuc manual.

Click to expand...

It would be an unusual machine with a Fanuc Control to not have a Block Delete function. There should be a switch on the Operator's panel to turn the Block Delete function On/Off. In your program a forward slash "/" is included at the beginning of the Block for those Blocks you wish to have the control ignore via the use of the Block Delete switch.

Regards,

Bill

My mistake. In all the hurry I was looking at DIAGNOSTICS instead of PARAMETERS.

Parameter 230: M code calling custom macro body O9020, setting value 006-255. It is set to 6.
If I understand this correctly, number set in the parameter is then M code for that subprogram. So if I put 007 in parameter 231, whenever I write M7, this will call O9021 sub program?

Manual says same as you, G20/G21 must not be switched during program. We use inch only for water pips, so this wont be an issue.

Parameter 10 is set to 10010000, setting it to 1000000 would unlock O9000 series programs as you say.


My logic behind programming the way I do? Got this machine, cleaned it, paint it and repaired few issues, had to figure out everything along the way. Same with programming. Boss told me to check for G-codes in a manual and then gave me a drawing and I had to write a program. With zero experience in CNC programming. At the beginning I was lost with tool offsets and how to set heights. Boss even wanted me to use G54-G59 for tools if couldn't figure it out because we were in a hurry. So as soon as heights were OK I started using that pattern. Bill you are the first that checked my code and pointed out this!

Regards,
Klemen

Hello kemenb,

kemenb said:

Parameter 230: M code calling custom macro body O9020, setting value 006-255. It is set to 6.
If I understand this correctly, number set in the parameter is then M code for that subprogram. So if I put 007 in parameter 231, whenever I write M7, this will call O9021 sub program?

Click to expand...

The setting value can be between 0 and 255 (excluding 98 and 99), not 6 and 255. The second part of your above statement is correct. Zero can be set, but does not call a Macro Program when M00 (Compulsory Stop) is specified. Zero signifies no M code being registered to call a Macro Program.

kemenb said:

Manual says same as you, G20/G21 must not be switched during program. We use inch only for water pips, so this wont be an issue.

Click to expand...

The Tool Change Macro is not the greatest I've seen. It records the Unit Mode of the control (G20/G21) in Common Variable #113, explicitly changes the Mode to G21 (Metric), then recovers the G20/G21 Mode of the control prior to the Tool Change, before exiting the Macro. And it does this for no particular purpose. If the Tool Change were to hangup, or for whatever reason you had to press the Emergency Stop, or Reset between the Tool Change Program changing the Unit Mode to G21 and where the Tool Change Program recovered the original G20/G21 mode, then the status of the control, in terms of the Unit Mode, may not be the same as before the Tool Change.

Its common practice to have a Safety Block as the first Block of all programs. This Block is designed to put the control in a Default state that is problem free for the program data that follows. The desired Unit Mode (G20/G21) always features in this Block.

With regards to your use of G43/G44, it like someone wanting to add the following Positive values.

A = 0
B = 5
C = A + B
C = 5

But instead of getting the answer as shown above, they say, that's not the way I'm going to do it. My system is going to be that I'm always going to change the sign of any number I want to add to another and then I'll subtract it as follows:

A = 0
B = -5
C = A - B
C = 5

The result are the same, just that one route is illogical.

Using G44 to apply Tool Length Offsets is like using the second method above to add 0 and positive five. You're using a Negative Offset value to have the tool Offset in a Positive direction and vice versa.

Its a dangerous practice of leaving out Tool Length Offset calls on the basis that you can't see the point in it. You will see the light the first time it causes a crash and you spend the next few hours/days fixing the mess. It's not a case of If its going to happen, but When it happens.

Regards,

Bill

Thank you for that! Now I know how to set heights and use offsets.

Is there a way to set machine so my absolute coordinate system will tell me the programmed position? For example if I use T3 and H3 Z would read Z-10 as programmed instead of some number (actual Z +/- offset). That number does not tell me much without adding or subtracting offset value in my had? I don't just want it to go to Z-10 and say its on Z-25.7, I want it to go to Z-10 and write Z-10 on the screen, and also repeat this on all G54, G55... Is it possible?
I would like to shift whole coordination system for offset value in Z direction. I know some machines do that. For example when you change tools on fanuc lathe with revolver it automatically shifts its coordinate system for tool offsets. And if you touch same spot with multiple tools it will read same coordinates in both X and Z direction.

Do you have any ode why if there is same tool already in the spindle as it starts the program with, machine would go down and back up uncontrollably?

regards Klemen

kemenb said:

Thank you for that! Now I know how to set heights and use offsets.

Is there a way to set machine so my absolute coordinate system will tell me the programmed position? For example if I use T3 and H3 Z would read Z-10 as programmed instead of some number (actual Z +/- offset). That number does not tell me much without adding or subtracting offset value in my had? I don't just want it to go to Z-10 and say its on Z-25.7, I want it to go to Z-10 and write Z-10 on the screen, and also repeat this on all G54, G55... Is it possible?

Click to expand...

Hello Klemen,
Yes its possible, settable via parameter.

kemenb said:

I would like to shift whole coordination system for offset value in Z direction. I know some machines do that. For example when you change tools on fanuc lathe with revolver it automatically shifts its coordinate system for tool offsets. And if you touch same spot with multiple tools it will read same coordinates in both X and Z direction.

Click to expand...

You can use G52 and the Shift value with the axis address to create a Child, or Local Coordinate System. Its cancelled by executing a Zero value with the specified axis address. G52 must be specified in Absolute (G90) mode.

kemenb said:

Do you have any ode why if there is same tool already in the spindle as it starts the program with, machine would go down and back up uncontrollably?

Click to expand...

You will have to publish an example of your program here to get an accurate answer to the above, otherwise its mere speculation.

Regards,

Bill

Do you by any chance know the parameter number or its name?

kemenb said:

Do you by any chance know the parameter number or its name?

Click to expand...

Hello kemenb,
I'm away from the office and don't have access to an OM parameter manual at the moment, so I can't tell you the exact parameter and bit. However, I do know that the parameter and bit for FS16 controls and above is 3104.6 and the bit name is DAL. The parameter will be different for the early OM control, but the bit name should be the same.

Regards,

Bill

Do you have a .pdf of Fanuc series O-MC, OO-MC, O-Maate MC manual, B-61404E/02?
I have an actual book at work but would like to have a copy at home, so I don't have to carry it back and forward.

There are no parameters in 3000 range, also didn't find DAL anywhere. I will check again later, maybe I just overlooked it.

Regards,
Klemen

Here is an actual program, written on 16.8.2014. As you can see it is not much different from what I've already written. I haven't had the chance to re write my programs.

O0085
G90 G55
M6 T2 /end mill 11,6mm
M3 S2200 F350
G0 X69,6 Y0
Z1
G1 Z-20,3
M98 P1002
X69,9 Y0
Z1
G1 Z-20,3
G0 Z1
M98 P1002
G56
X69,9 X0
Z1
G1 Z-20,3
G0 Z1
M98 P1002
X36,9 Y0
Z1
G1 Z-20,3
G0 Z1
M98 P1002
M6 T3 /T-mill 14mm
M3 S1600 F80
G56
G44 H3
X36,9 Y0
M98 P1003
X69,9 Y0
M98 P1003
G55
X69,9 Y0
M98 P1003
X36,9 Y0
M98 P1003
M6T4
G44 H4 /2-cutter end mill 5mm
M3 S2000 F300
G0 X13 Y0
Z1
G1 Z-20,3
G0 Z30
G56
Z13 Y0
Z1
G1 Z-20,3
G0 Z30
Z200 Y190
M30

O1002
G91 F200
X-1,65
G2 X3,3 Z0 Z-2,5 R1,65
G2 X-3,3 Z0 Z-2,5 R1,65
G2 X3,3 Z0 Z-2,5 R1,65
G2 X-3,3 Z0 Z-2,5 R1,65
G2 X3,3 Z0 Z-2,5 R1,65
G2 X-3,3 Z0 Z-2,5 R1,65
G2 X3,3 Z0 Z-2,5 R1,65
G2 X-3,3 Z0 Z-2,8 R1,65
G2 X3,3 Z0 R1,65
G2 X-3,3 Z0 R1,65
G90
F380
G0 Z30
M99

O1003
Z-5,7
G91
G1 X-3,2
G2 X6,4 Y0 R3,2
G2 X-6,4 Y0 R3,2
X3,2
Z-4,52
X-3,2
G2 X6,4 Y0 R3,2
G2 X-6,4 Y0 R3,2
X-3,2
G90
G0 Z30
M99

The other day I turned machine on to mill openings on small plastic boxes and feed hold or feed rate 0-150% would not work. Rapid traverse selector worked (had it at 25%) but work feed selector did not work, machine operated at 100% of set value. Then I wanted to change tools and tool magazine (umbrella) got stuck under the spindle, giving me an error "not fin" so I turned machine off and back on to release pressure in tool magazine pneumatic. After that feed hold and feed rate selector worked. These little glitches are getting very annoying. What could be wrong with my machine? Faulty circuit? Bad contacts?

Regards,

Klemen