Marposs probe on VMC4020 w/ Fanuc 18iMB5

[XYZ machine]

Installing a touch probe on our 4020. Cant seem to get any clear answers on if there is a "M" code to "turn the probe on or not. I have high speed skip and also custom macro options enabled. The JA40 connector is where the skip channel is at. When I initiated a G31 G91 X-1.0 F10.0 nothing happens. No table movement, I was going to touch the probe to see if it would stop the axis. Guys any help would be greatly appreciated, I bought this stuff new on the shelf for about 1/6 of what it should cost, bought my software from Marposs.

HELP HELP HELP.......................

XYZ

Similar Threads:

• marposs probe
• vmc4020/cnc88HS probe
• digitizing with Marposs probe
• Fanuc 18iMB5 assistance
• Marposs T25 probe problems

[Al_The_Man]

An M code to turn the probe on is usually only if the probe has a centrifugal switch etc, not to activate the G31, if the G31 option on the control is active, then normally all that is required is to trip the skip input, if the G31 line does nothing, It could be two things.
1/ the G31 option is not present.
2/The other is if the probe logic is wrong and the probe is initiating a skip right off the bat. If it drops through to then next line then this is the problem.
Al.

[XYZ machine]

I noticed that regardless of the x or y value the axis only moves like .0026 when I send the G31. Pulled the power off the interface board and tried the G31 with same results. I dont get an error when I execute a G31 and Fadal said the option is on the machine. Just cant figure out what I'm doing wrong or maybe I'm not. I have not loaded the Macro software on yet Marposs calls out parameter 2201 "Controlling machine stop in single blk by macro command"
Well it not on my control thats a Digital axis servo parameter. So I have to let them know about that. Thought this would be simple but it's looking to be a pain.....

Thanks,
XYZ

[Al_The_Man]

Parameters 6200 to 6220 also configure the skip.
Al.

[XYZ machine]

I went down the list from 6200-6220 channel HD0 is the one I would use and is active. I have unhooked the interface and the machine still wont execute the G31 G91 X1.0 F5.0, it moves about .002 and it stops. The Fanuc tech said maybe Fadal has a low speed skip on and its getting it signal there. Frustration sets in further, my good deal on the equipment is turning into a nightmare........................

[Al_The_Man]

How is 6200 and 6201 set? IIRC if the skip signal input is open it performs a skip.
After the G31 line moves .002, does it fall through to the next line?
I think the low speed skip is a PMC input, something like input X004 comes to mind.
Al.

[XYZ machine]

6200 is 1 0 1 1 0 0 0 0

6201 is 0 0 0 1 0 0 0 0

There is no next line I was simply punching in the G31 g91 x1.0 f 5.0 on one line. If I reached out and touched the probe it should halt the X axis, if I do nothing it should complete the X 1.0 incremental move at a feed of 5.0 IPM. I do nothing at all except hit cycle start and it moves like .002 in the X and thats it. I am not even attempting to load the Marposs macros until I can test the skip function correctly.

XYZ

[Al_The_Man]

What I meant was that if somehow the skip is activating on cycle start, if you have another line after the G31 and it drops through and carries out that line then this it what is happening.
You could also try setting bit 6 of 6200 to 1 SRE and see if there is any difference.
Al.

[XYZ machine]

Input:

g31 g91 x1.0 f5.0
y1.0 f10.0

It read thru and made the "Y" move.
XYZ

[Al_The_Man]

Does that mean the skip worked or just that it immediately fell through to the second line?
Al.

[XYZ machine]

Sorry Al,

the skip did not work but it did read thru.

I did not change the 6200 para as of yet.

Thanks,
XYZ

[Al_The_Man]

I did not change the 6200 para as of yet.

That could make a difference, are you inputing to JA5 high speed input option? As the High speed inputs are direct into the NC side and not the PMC side the status of the high speed inputs can be seen on parameters F122 bits #7~#0.
I think you should also see a captured positions in macro var 5061 ~ 5063
Al.

[XYZ machine]

Inputting on the JA40 connector which goes to a terminal block on the Fadal TB2, which I am going to use Channel HD10. I'll change that para after this cycle ends on the machine and see what happens.

XYZ

[XYZ machine]

Well I changed the 6200 para bit 6 to on, that did infact let it now execute the g31 g91 x1.0 f5.0.

So I hooked up the two wires from the Marposs interface card to HD10 channel, executed the same code line with the probe in the spindle. Hit cycle start x axis moves and I touch probe tip but it did not halt the axis it kept going.

AL you have shed some light in a positive direction, I finally feel somewhat good about this now!!!

Keep pushing me along I know we can get it now!!!!

XYZ

[Al_The_Man]

It would seem to me that the contact closure is not happening, I don't know what the configuration is of the Marposs card but just to make sure the skip is working, I would hook up a simple switch or pushbutton to the HDI0 input and the associated ground connection (next pin) and run the test program and operate the push button to simulate a probe trip, if it drops through again on cycle start , just reverse the bit 6 or use a normally closed PB instead of N.O.
If that works then you will have to find out what type of interface output the Marposs card has.
Al.

[XYZ machine]

Hooked up momentary push button to verify if I could stop axis after g31, and it works every time!!!

I then looked up the Probe 1 N/O SSR contact on the wiring diagram from Marposs and hooked it into HD10 channel, and it now works with the probe.

I have another problem that I did not mention before but I had changed my Halogen Flood work lites to Flourecent and guess what the probes receiver thinks its a signal..............any ideas on that?

Also is the probes accuracy dependant on the feed rate of the axis, I know I fed at 5.0 ipm it stopped in one place, then fed at 10.0 ipm and it stopped differently. Seems to repeat within a few tenths but diff location.

Sorry for so many questions this is all new to me, never used probing before in all my years operating and programming CNC's............... (28)

XYZ

[Al_The_Man]

I have never come across this with flourecent's, I wonder if a different color tube would make a difference.
The typical measuring sequence is to make the first probe trip with G31 at a high feed rate and then back off the distance equal to the hysterisis of the probe. (till it opens again). and then come in again at a creep feed rate for the actual measuring.
Most probe manufacturers have macros for all various measurement configurations, and it is worth while getting a copy, or get a copy for any make and adapt.
The true test is not where the axis stops, but what was captured in the H.S. skip macro variables.
Also you never use an unprotected move with a probe, IOW if you are just moving the probe to an initial rapid position, it should contain a G31 in case of collision.
Al.

[XYZ machine]

Good point about what the skip capture was and not the actual axis position! I had just read about always include a g31 on the line when positioning a probe. I have Marposs macro part check software. Just have not loaded it in the machine yet. I will try to keep you informed of further developments! Hopefullythis thread will be able to help others.

XYZ

[Shizzlemah]

In addition to a G31 on any motion line, also do a position check to be sure your spindle moved about as far as it should have so you can be sure you got where you wanted to go.

I Crunched a Renesahaw last month and I'm a little paranoid now!

Standard probe routine for me is:

G90 G31 Xwhatever F50.0 (move at 50IPM until touching)
G91 G1 G31 X+.005 F10.0 (move .005 past a touch)
G91 G1 G31.1 X-.100 (move until probe is not touching)
G91 G1 G31 X-.010 (move .010 past probe clear)
G90 G31 Xwhatever F1.0 (final touch to capture)

[XYZ machine]

Not questioning but trying to understand !!

Why did you make the +.005 inc move after touch.

After backing up inc -.100, why inc move another -.010. would it have not been the same as a -.110 inc move anyway??

The feed move at 1.0 ipm is understood to be final touch.

I assume you are not using any software ie: Renishaw or Marposs for part pick up macros??

Thanks,
XYZ