Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

FAnuc inspection post

7 REPLIES 7
Reply
Message 1 of 8
paulo2Z36L
311 Views, 7 Replies

FAnuc inspection post

Hi,

 

I need info about this error in the inspection fanuc post. somehow a cam parameter (i assume) is not read correctly and it outputs code that the machine won't read.

....

(GEOMETRY ONLY)
N65 #8=#[2000 + #4111]
N70 #1=[[#500 + #501]/2]
N75 #9=PRM[6014,4]  <---------- this liene causes me trouble....don<t know why is wont get a value
N80 IF [#9 EQ 0] GOTO90
N85 #8 = 0
.....
 
thank you
7 REPLIES 7
Message 2 of 8

Hi @paulo2Z36L 

That's all about the tool length, first thing I notice is you have the post property "Tool offset Type" or something like that. Set to Geometry only. Possibly your machine has 2 columns on the tool offset page. If you have 2 columns, one for geometry and one for wear then please set that post property to "Geometry and Wear"

Give that a go and let me know how you get on.



Richard Stubley
Manager - Manufacturing Specialist Team
Message 3 of 8
paulo2Z36L
in reply to: paulo2Z36L

Hi,

 

Juste tried it....

I keep geting the same error. 

 

(GEOMETRY AND WEAR)
N65 #8=#[2000 + #4111] + #[2200 + #4111]
N70 #1=[[#500 + #501]/2]
N75 #9=PRM[6014,4]
N80 IF [#9 EQ 0] GOTO90
N85 #8 = 0
 
Below is a is a copy paste from of post...see section in bold.
 
 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);
  }
}

function inspectionProcessSectionEnd() {
  // close inspection results file if the NC has inspection toolpaths
  if (inspectionVariables.hasInspectionSections) {
    if (getProperty("commissioningMode") && inspectionVariables.printParameterCheck) {
      forceSequenceNumbers(true);
      writeBlock(inspectionVariables.macroVariable1 + "=PRM[6019,3]"); <----- tihs one here seem to be read...somehow
 
basically it's checking for a tool lenght offset at 0. Maybe i could use a #2200 parameter...
 
This is for a M80 control, fanuc compatible.
 
 
Message 4 of 8

Hi,



Just tried it....

I keep geting the same error.

(GEOMETRY AND WEAR)
N65 #8=#[2000 + #4111] + #[2200 + #4111]
N70 #1=[[#500 + #501]/2]
N75 #9=PRM[6014,4]
N80 IF [#9 EQ 0] GOTO90
N85 #8 = 0

Below is a is a copy paste from of post...see section in bold.

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);
}
}

function inspectionProcessSectionEnd() {
// close inspection results file if the NC has inspection toolpaths
if (inspectionVariables.hasInspectionSections) {
if (getProperty("commissioningMode") && inspectionVariables.printParameterCheck) {
forceSequenceNumbers(true);
writeBlock(inspectionVariables.macroVariable1 + "=PRM[6019,3]"); <----- tihs one here seem to be read...somehow

basically it's checking for a tool lenght offset at 0. Maybe i could use a #2200 parameter...

This is for a M80 control, fanuc compatible.
Message 5 of 8

Hi @paulo2Z36L 

It just checks for wether the tool length is already accounted by the machine or not if we call the #5063 variable.

you can disable this check in the post as most of the machines will include the tool length compensation value when we call #5063.

Edit the post and find for this line in the post 

toolLengthParameterCheck       : true,

and set it to false

toolLengthParameterCheck       : false,

 

this should not output the PRM section of codes in the nc

 


Boopathi Sivakumar
Senior Technology Consultant

Message 6 of 8

Hi @paulo2Z36L out of interest what is the error you are getting on the machine?

 



Richard Stubley
Manager - Manufacturing Specialist Team
Message 7 of 8

Sounds good. I will give it a try.

It's only when i use inspection surface on fusion, all other probing strategies work just fine.

thank you
Message 8 of 8

Hi,

Machine will give we '' unpaired brackets error''.

i tried to see what this parameter was for ans pulled out all the documententation....and it seems that it's nowhere used....

This occrurs only when I use the Inspection surface option, other options seem to work just fine (bore, web, etc).

I will disable this conftions, as per susgested above. Or I'll just ut in my machine active length parameters. It only for the DPRNT block, from what I see. My built in macros fro probing work just fine using the the active tool lenght.

I'll get back to you guys, as it might become handy for someelse using Mitsubishi M80/M70 controls or Fanuc 16-18-20. Mine is

Thank you

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report