Fanuc inspection post

[paulo2Z36L]

Hi,

I'm trying to do some Surafce inspection.

When I use the Fanuc Inspection post....it seems that a certain parameters (cam parameter I guess) is not read.

Basically it check for feed value if it's equal to 0.

see below the sample program

....

(GEOMETRY ONLY)

N65 #8=#[2000 + #4111]

N70 #1=[[#500 + #501]/2]

N75 #9=PRM[6014,4]     (<-----this line right here is causing me some trouble)

N80 IF [#9 EQ 0] GOTO90

N85 #8 = 0

...

thanks for you help

@Richard.stubley 

[serge.quiblier]

Hi @paulo2Z36L 

what is the controller version? 16, 18, 30?

Because the PRM function in not available on all controllers.

It is used for checking a parameter on the machine to dertermine in which coordinates sytem the probing location will be returned by the controller. (local workplane versus machine reference)

Maybe your controller does not support this.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[paulo2Z36L]

Hi,

My controller is a Mitsubishi M80. I always use fanuc post for these as they are, most of the time, compatible.
I guess I dont have this availble then.

You know where I could find the documentation for these PRM fonctions?

I will find my way around it.

thank you

[serge.quiblier]

Hi @paulo2Z36L 

Your post seems to be an older copy, as it has been fixed recently, and in fact the parameter that need to be checked is that one:

This is the real Fanuc parameter.

I have not idea if Mitsubishi is using the same number and have the same functionnality.

In the Fanuc manual, the PRM[] function is explained in the macros commands.

Again, I make no assumption that ta similar function exist in the Mitsubishi post.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[paulo2Z36L]

Hi,

I change this: toolLengthParameterCheck : true, to flase and it seems to work.

Not sure why work coordinates it checked here...or maybe I'm not following...

here's the line of code that is problematic (copied from the post):

isDPRNTopen = true;
if (inspectionVariables.toolLengthParameterCheck) {
forceSequenceNumbers(true);
writeBlock(inspectionVariables.macroVariable1 + "=PRM[6014,4]");
writeBlock("IF [" + inspectionVariables.macroVariable1 + " EQ 0] GOTO" + skipNLines(2));
writeBlock(inspectionVariables.activeToolLength + " = 0");
writeBlock(" ");
forceSequenceNumbers(false);

I tried the new version available on the Autodesk site....other than that, my Fusion is up to date.....where could I find the a newer version?

Thnak you
@Richard.stubley

[serge.quiblier]

Hi @paulo2Z36L 

I am a post author, so I have access to our repository that will be used to generate the online library.

That library is publicly updated every Monday.

So, I can see some changes before they are pushed to the public.

But it will not solve your problem, and the same PRM function will simply be reading another variable.

So, if PRM does not work on your controller it will solve nothing.

Is this a 3-axis machine, or a five-axis machine?

Because on a 3-axis machine checking the parameter 6014/5400 is useless.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[paulo2Z36L]

Hi,

It's for a 3 axis machine. I cancel this parameter check and it works fine....just need minor modification for the PCLOS and for the DPRNT format...somehow it wont read the DPRNT[TOOLPATHID*#20[54]]. Maybe it doesn'like the two brackets....i'll tru to put a ''*''. EDIT: fINALLY FOUND IT.... MACHINE TAKES ONLY [44]...DONT KNOW WHY IT SHOOTS [54] IT ONLY TAKES 8 DIGITS...JUST HERE THAT I GOT THE [54]...ALL OTHER HAVE [44]. 

IF THERES A SWITHC OR MACHINE CONFIG TO SAYS ITS A 3AXIS MACHINES....I'D LIKE TO KNOW WHERE I COULD FIND IT...ON THE MACHINE CONFIG SIDE OR IN THE POST.

(INSPECT2)
G00X1.4985Y-0.1702
DPRNT[END]
PCLOS
PCLOS
POPEN
DPRNT[START]
DPRNT[RESULTSFILE*INSPECT2-RESULTS]
DPRNT[DOCUMENTID*9D0840D5-CE96-4530-B6CB-CF0C3FA00874]
DPRNT[MODELVERSION*6BAA9A11-57B3-4963-9C5A-C2BD9FC389D6]
#20=7
DPRNT[ TOOLPATHID*#20[54]]<--MAYBE THE FORMAT HERE...MACHINES READ ALL OTHER EXCEPT THIS ON
DPRNT[ TOOLPATH* INSPECT2]



My next step is to do the same on my 5 axis (mazak c600) on a tilted plane....so i might need to do this check prior...

In the end I was able to send my date in Fusion and compare. Only two points out of four were imported...may be because of my edit on the file on the control side.

other then taht, the post is awesome!

Thank you

[serge.quiblier]

Hello @paulo2Z36L 

I don't know if/why the system would be choking on [54] as the manual for Mitsubishi M80, M800 (common) show this as possible:

There is no switch in the post for 3 axis or 5 axis.

But to generate 5 axis code, the post must know the kinematic of the machine.

It can be provided by a machine definition file.

Another solution is to hand edit the post processor and define the kinematic in it, but it's not the recommanded way.

It it easier to create and edit a machine definition file in the machine library.

Then assigning this machine in the setup, or else using it when posting the code, in the NC Program dialog.

For the tests on the mazak machine, I would suggest try that post processor:

Link to the beta post for Mazak inspection. 

Because using the Fanuc post may also cause issue on Mazak.

Let's be clear about something:

Yes, Mitsubishi, Mazak, Fanuc may have pretty close G code, that can be run from one controller to another without too much hassle.

But the internal layout of the controller is totally different, for example the parameters are NOT the same between the brands.

So, the PRM function will not exist, and the parameters are completely differents. Fanuc is a single set ranging from 20 to over 19000. Mazak have several groups, like the F parameters, the the G parameters , etc....

As said previously, for 5axis machine, a machine definition file, describing the rotary axes configuration is needed.

About the missing points in the result file.

Make sure to run the code without machine warning or error.

When finished, before importing in Fusion, open the result file with a text editor.

Locate the latest START tag in the file.

If you probe four points, there should be 8 lines alterning G330 and G331, till a END tag.

If not, then a problem occured during the process.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[paulo2Z36L]

hi,

HI, everything works now...been running a few parts and I imported the data in Fusion. I checked my results with my cmm and it works like I wanted.

For the M800, here is what I found...just the page before the one you pasted here.
I can really copy paste here. But it says significant digits above (d1) and after (c1) the decimal point shoulb be as follows: c+d <=8.

I'll try the mazak insp post later.

Thank you, much appreciated.