[banshee1a]

Been trying to creata a small macro program for our small horizontal mill to send the machine to its APC position and execute a pallet shuttle. The machine is a Jenso with an 18iMB control. I want it to execute using a G100 call. We have an Okuma 630H horizontal set up this way and I want the Jenso machine to match. I made the program the same on the Jenso, but I get an "Invalid G code error" every time I try it. I made a subprogram for our thru the spindle coolant, due to the fact that it takes 2 M codes to turn it on to use M150 to turn it on. I tried to make it a macro program, but I kept getting an error, so I changed the O word to match for a subprogram call and it worked fine. Can somebody clue me in on what I might be missing? Thanks a bunch guys.

[g-codeguy]

I originally used G100 to call my barfeed operation up when we got our first Hardinges. These were OT controls. When we got new ones with the 18T controls, I was unable to use G100, so I had to switch my programs to a different call number. Don't know why. I supposed it was due to the way the manufacturer set the machine up.

[stevo1]

What you have to do is set up the G100 call in your custom macro parameters. I believe that for the 18i control they are parameters 6050-6059 calling programs 9010-9019
ex.
6050 calls program 9010
6051 calls program 9011
...
6059 calls program 9019


Activate parameter write enable which you should see when you press your Offset/Settings key. You have to be in MDI to change. Go to parameter 6050 and set it to 100. This will call program 9010 everytime you command a G100. Depends on what program number you want you can set parameter 6051 and it will call program 9011 ect. Remember you have to unlock your 9000 programs in order to create the program you want.

Stevo

[banshee1a]

Yup, thats what I tried stevo1. Every time I cycled a G100 I get a "010 improper g code" message. Our Okuma with a 16i control runs it no problem. If we call up that prg and run it in auto, the prg. executes fine. Now somewhere I've read that you need to register G codes, but I'm not sure what that means. I even changed it to a G35 to see if there was a limit on how many numbers your allowed after the G, but that didn't work either. Any other ideas.

[stevo1]

Are you sure that you have MacroB programming option in your control?? Try going to MDI and type #100=5/EOB/Cycle start. If you get an alarm you probably don't have the option. If you have it you can look at variable #100 it should be equal to 5.

If you do have macro B see if your M codes work for calling a macro.

(set 1)
Parameters
6071 calls program 9001
...
...
6079 calls program 9009


(set 2)
Parameters
6080 calls program 9020
...
...
6089 calls program 9029

Let me know what you get.
Stevo

[g-codeguy]

Yup, thats what I tried stevo1. Every time I cycled a G100 I get a "010 improper g code" message. Our Okuma with a 16i control runs it no problem. If we call up that prg and run it in auto, the prg. executes fine. Now somewhere I've read that you need to register G codes, but I'm not sure what that means. I even changed it to a G35 to see if there was a limit on how many numbers your allowed after the G, but that didn't work either. Any other ideas.

Have you tried calling Fanuc? Doesn't affect me anymore, but I am curious as to the problem. Tried the G100 on 3 machines and it worked. Not about to try every one until I find the one it didn't work on.

stevo1, I didn't realize that Macro B had to be active to use parameter 6050, etc.

[stevo1]

g-codeguy I am not 100% that you have to have macroB in order to use the 6050 parameters, but they are "Custom Macro" Parameters. I have always had Macro programming and I have never run across a problem like this that would not let you set custom G&M codes. Thats why I asked him to try the Mcode parameters and try a quick test in MDI to see if he does actually have Macro capability. If he does not have macro programming it would lead me to believe that this is the problem. If I get time today I will shut my MacroB option off on one of my controls and try some of the custom G&M codes I set up and see what happens.

Stevo

[g-codeguy]

Stevo[/quote]

g-codeguy I am not 100% that you have to have macroB in order to use the 6050 parameters, but they are "Custom Macro" Parameters. I have always had Macro programming and I have never run across a problem like this that would not let you set custom G&M codes. Thats why I asked him to try the Mcode parameters and try a quick test in MDI to see if he does actually have Macro capability. If he does not have macro programming it would lead me to believe that this is the problem. If I get time today I will shut my MacroB option off on one of my controls and try some of the custom G&M codes I set up and see what happens.

Stevo

You are probably right. I had forgotten the 6050 series were part of the Macro B section. Like you, all our lathes (with Fanuc controls) have Macro B. Maybe I made a stupid mistake the first time, but I know one of the lathes wouldn't except G100 in parameter 6050. However it is very possible it was my fault.

Should say that I had 100 in 6050 (I think ), but control alarmed when I called it with G100. Doesn't really matter now as I've been using G200 for several years now. I was only curious as to what is causing banshee's problem in case I every came across it again.

[banshee1a]

Sorry for not replying sooner guys. For some reason after I posted my question, the site said my account needed to be activated and it wouldn't let me do anything. Seems fine now. My boss said we were supposed to have MacroB, but I had tried previously to create one using an M code before I posted my question, and that one woudn't work either. Is their a way to turn on MacroB? Assuming the vendor just didn't turn it on/enable it. My boss told me he thought it was supposed to be there. I appreciate your help guys. I haven't tried your suggestion stevo1 as the machine has been running, and I didn't want to stop it. We are going to be getting a software upgrade from Fanuc sometime soon to fix the offset table layout, so maybe that may fix this and some other problems we are having with the control. Thanks again guys.

[stevo1]

Using the MDI method as I explained before is the easiest way to check to see if you have MacroB in your control. I am not 100% sure of how to active options on the 18 controls. PM me your 9900's and I can tell you if you have it turned on or not.

How old is your control. The newer controls (i think within the last 1-2 yrs) do not have to ability to change the option parameters. I believe that Fanuc has headed that off.

If you already have Fanuc coming to your facility then you might want them to look into it. They will beable to tell you if MacroB was purchased from them for that control. If it was and it is not turned on then they should turn it on for you. If it was not purchased then you would have to buy it. I think it is pretty pricy$$(nuts)

Stevo

[banshee1a]

The machine is an '06, but we just got it a couple weeks ago. So the control is only a couple years old. The machine is up and running right now so I can't check the 9900's, but when I was looking last week I don't think I saw anything in that range, and I to had heard that Fanuc has started blocking that range. I'll guess I'll have to wait until they get here to get the final word. Thanks for the help steve01.

[g-codeguy]

You don't have to stop the machine to check what various parameters might be set at. At least I don't have to with any of our machines, mill or lathe. Changing one is, of course, another matter.

[banshee1a]

You don't have to stop the machine to check what various parameters might be set at. At least I don't have to with any of our machines, mill or lathe. Changing one is, of course, another matter.

If the machine's running our policy is to not interface with the control, plus I don't like to disturb the operator, and change their routine/habits ( I hated that when I used to run machines). There also isn't nowheres near enough time to write the codes down before the operator has to use the control in some way. But anyhow I was finally able to download all the parameters today. Our machine vendor told me today that to use the "Macro call using G code" function, you don't have to have macro programming, but I still can't get it to work. Anybody else have any more ideas?

[banshee1a]

Figured out which parameter controls the macrob programming and it is turned off on the Enshu, but is turned on on our Okuma. I am able to turn it off on the Okuma, so I did that today and the G100 failed to work, so apparently you do need macroB to use the 6050 series parameters. So much for the machine vendors. They quoted us around $2700 I think just to enable it. I need to look at the parameter inspection list supplied by Fanuc for that control to see if it was initially turned on, and then the vendor turned it off to charge us for it again. This has happened to us before. I do remember seeing that some of the 9900 parameters were changed, but right now I don't remember which.

[BluegrassPicker]

Yes Fanuc has started a "rolling password". The Fanuc tech has to get the password and when it is entered in the control, an internal timer starts. The password is only good for 24hrs.
We have an A61 Makino with the Pro5 (windoze) POS. The software had to be upgraded shortly after being installed. The tech had to get 3 passwords to finish the job.

[stevo1]

Banshee1 you have a PM

[gbowne1]

Are you sure that you have MacroB programming option in your control?? Try going to MDI and type #100=5/EOB/Cycle start. If you get an alarm you probably don't have the option. If you have it you can look at variable #100 it should be equal to 5.

I just tried this today on my 18i and it works. I never really noticed that i had this option. The person who set up my 18iMA loaded his custom parameters into the machine.

Lately I have been playing with it. In the midst of my control builds and finishing building machines, I've had time to work on some projects.. inclduding getting on with this particular control.

I read the machining center operation manual for the 18i. '

The machine has scales from Mitutouyo AT553-150-SC.. and

Parameter 3111.0 is "1".. and been playin with the page in System, arrow over to the SRV.PARA then to SRV.TUN. I'm thinking about having a look at DGN #300. I hope I don't have some scale or servo mismatch, because at times I don't think its following correctly.

It has 3 of the Alpa SVM1-20 A06B-6096-H102 & one A06B-6114-H205 servo ampls. The 6114 runs the 4th axis.. although I thought about changing this.

Greg