Too fast for Fanuc

[Leon82]

Has anyone noticed with the PC based Fanuc your mdi lines are filled with random characters?

 

Well if you type too fast it happens

[cncappsjames]

"...PC Based...".

You're going to need to elaborate a little bit. Are you talking about the "Panel i" interface or the "iHMI" interface or something different all together? 

[Leon82]

15 minutes ago, cncappsjames said:

"...PC Based...".

You're going to need to elaborate a little bit. Are you talking about the "Panel i" interface or the "iHMI" interface or something different all together? 

It happens with the manual guidei interface and ihmi with windows in the background. 

[cncappsjames]

Can you post a screenshot of the interface? 

[Leon82]

[cncappsjames]

When I get in the office Monday I'll check out our MX-330 and see if I see anything unusual. 

You know you don't have to use "O" number for programs anymore right? You can use up to 32 Alphanumeric characters; 0-9, A-Z, - and _. You can't uses spaces and other reserved characters. Upper and/or Lower Case letters are OK as well. This goes for all 30i, 31i, 32i, and 0i-F series controls. 

See how your "Feed" indicator has a metric number? You want to know where to fix that? 

Thanks for the info. 

[Leon82]

18 minutes ago, cncappsjames said:

When I get in the office Monday I'll check out our MX-330 and see if I see anything unusual. 

You know you don't have to use "O" number for programs anymore right? You can use up to 32 Alphanumeric characters; 0-9, A-Z, - and _. You can't uses spaces and other reserved characters. Upper and/or Lower Case letters are OK as well. This goes for all 30i, 31i, 32i, and 0i-F series controls. 

See how your "Feed" indicator has a metric number? You want to know where to fix that? 

Thanks for the info. 

Yes and yes I wouldn't mind knowing how to switch that.

I think it may be there is a fraction of a second there are 2 buttons pushed from my ninja like reflexes.  So my code sometimes looks like this. G)0 G)x)yo

I have been waiting for 6 months for the parameter to prevent the  100+ macro variable from clearing at m30. Do you happen to know that.

[balnh]

Try parameter 6001.6 set to 1 to retain variables. 

[cncappsjames]

Here's the parameters I change on all of our FANUC 30i and 31i- controlled 5-Axis machines; 

#1300.1 = 1 Handle Jog OT alarm not output. (NAL)

#1401.4 = 1 Rapid Stops when Feed Override is at 0% (RF0)

#6001.3 = 1 Output all MACRO Variables on punch (PV5)

#6001.6 = 1 #100-#199 not cleared on reset. (CCV)

#6005.0 = 1 In Sub Program Call use Sequence Number (SQC)

#6019.0 = 1 Output all variables as decimal number (MCO)

#11350.1=1 Current section of program only displayed, not look ahead section (APD) (Requires Reboot)

#11351.6=1 Parameter Group Names Displayed (GTD)

#11775.0=1 Smooth TCP is Active  (TP2)

#13265 = 999 (MAX TLO Available) Tool Life Management H Offset Number (0=99)

#13266 = 999 (MAX TLO Available) Tool Life Management D Offset Number (0=99)

#13451.1 = 1 TWP 0's ok. (ATW)

#14854.6 = 1 Program Input/Output is enabled during Background Editing (BGO)

#19746.4 = 1 (TBP) G41.2/G42.2 ok

 

This should set you up nice. 

[Leon82]

Thanks.

 

Does the last one mean can use cutter comp on 5 axis circle mill?

[cncappsjames]

1 minute ago, Leon82 said:

Thanks.

 

Does the last one mean can use cutter comp on 5 axis circle mill?

Yep. 3D Tool Comp. When you use CAMplete and you program a 5-Axis toolpath that has Wear/Computer/Control Comp options, you'll get G41.2/G42.2 output.

[Leon82]

3 minutes ago, cncappsjames said:

Yep. 3D Tool Comp. When you use CAMplete and you program a 5-Axis toolpath that has Wear/Computer/Control Comp options, you'll get G41.2/G42.2 output.

Nice, we get an alarm at the machine currently but I will try it

 

Thanks!

[cncappsjames]

That will get rid of the alarm as long as your machine has the option. If you're in the US, I believe they all come with it.

 

When I get to the office Monday, I'll get the setting change to fix the feed rate indicator. It's a FANUC issue. They fixed it in subsequent software releases. That value didn't scale when in Inch/Metric mode. 

[Leon82]

1 minute ago, cncappsjames said:

That will get rid of the alarm as long as your machine has the option. If you're in the US, I believe they all come with it.

 

When I get to the office Monday, I'll get the setting change to fix the feed rate indicator. It's a FANUC issue. They fixed it in subsequent software releases. That value didn't scale when in Inch/Metric mode. 

Our 330 has the same thing and they had to do an update and now it's good.  That pic is our pc4

[cncappsjames]

It's the same setting to change on the PC4. There's a text file to edit. I just can't remember which one off the top of my head. 

[Colin Gilchrist]

6 hours ago, cncappsjames said:

Here's the parameters I change on all of our FANUC 30i and 31i- controlled 5-Axis machines; 

#1300.1 = 1 Handle Jog OT alarm not output. (NAL)

#1401.4 = 1 Rapid Stops when Feed Override is at 0% (RF0)

#6001.3 = 1 Output all MACRO Variables on punch (PV5)

#6001.6 = 1 #100-#199 not cleared on reset. (CCV)

#6005.0 = 1 In Sub Program Call use Sequence Number (SQC)

#6019.0 = 1 Output all variables as decimal number (MCO)

#11350.1=1 Current section of program only displayed, not look ahead section (APD) (Requires Reboot)

#11351.6=1 Parameter Group Names Displayed (GTD)

#11775.0=1 Smooth TCP is Active  (TP2)

#13265 = 999 (MAX TLO Available) Tool Life Management H Offset Number (0=99)

#13266 = 999 (MAX TLO Available) Tool Life Management D Offset Number (0=99)

#13451.1 = 1 TWP 0's ok. (ATW)

#14854.6 = 1 Program Input/Output is enabled during Background Editing (BGO)

#19746.4 = 1 (TBP) G41.2/G42.2 ok

 

This should set you up nice. 

[#Rekd™]

16 hours ago, cncappsjames said:

Here's the parameters I change on all of our FANUC 30i and 31i- controlled 5-Axis machines; 

#1300.1 = 1 Handle Jog OT alarm not output. (NAL)

#1401.4 = 1 Rapid Stops when Feed Override is at 0% (RF0)

#6001.3 = 1 Output all MACRO Variables on punch (PV5)

#6001.6 = 1 #100-#199 not cleared on reset. (CCV)

#6005.0 = 1 In Sub Program Call use Sequence Number (SQC)

#6019.0 = 1 Output all variables as decimal number (MCO)

#11350.1=1 Current section of program only displayed, not look ahead section (APD) (Requires Reboot)

#11351.6=1 Parameter Group Names Displayed (GTD)

#11775.0=1 Smooth TCP is Active  (TP2)

#13265 = 999 (MAX TLO Available) Tool Life Management H Offset Number (0=99)

#13266 = 999 (MAX TLO Available) Tool Life Management D Offset Number (0=99)

#13451.1 = 1 TWP 0's ok. (ATW)

#14854.6 = 1 Program Input/Output is enabled during Background Editing (BGO)

#19746.4 = 1 (TBP) G41.2/G42.2 ok

 

This should set you up nice. 

Just plain bad a$$ help James!!! Thank you for coming back to help others!!!!

[cncappsjames]

Ok @Leon82,

1. Press the button that has 9 filled boxes (looks like a negative of Tic-Tac-Toe)
2. Press File Manager on the touchscreen. This brings up Windows Explorer
3. On the left pane of explorer scroll down to the D:\ drive and double tap on it
4. Navigate to D:\FANUC\iHMI\MTB\CNCOpera\Setting
5. Double tap on Setting_Data.txt open with Word Pad (or notepad if you prefer)
6. Scroll down to the following;

[Actual_Feedrate]

Max_Scale-Markings_Val=40000

Change 40000 to 1575

Tap File, Save, and save the file. 

Close out of Word Pad (or Notepad). Close out of Explorer. Navigate back to your CNC screen. You may need to go to another screen to get the display to refresh. Hope that helps. 

 

As to the keyboard not keeping up... I guess I type slower. LOL I did notice the computer doesn't seem to be quite as responsive as a dedicated PC or dedicated CNC. I'm going to do a little more testing between Christmas and New Years and see what I can figure out. 

 

 

[cncappsjames]

@Leon82, do you use the "Favorites" function in MDI mode? 

[Leon82]

15 minutes ago, cncappsjames said:

@Leon82, do you use the "Favorites" function in MDI mode? 

Yes,

 

I have a few touch off macros saved and shutdown also

[cncappsjames]

That's a great feature. It's easier to use than the old Manual Guide i  cycles you can save. 

[balnh]

6 hours ago, cncappsjames said:

Ok @Leon82,

1. Press the button that has 9 filled boxes (looks like a negative of Tic-Tac-Toe)
2. Press File Manager on the touchscreen. This brings up Windows Explorer
3. On the left pane of explorer scroll down to the D:\ drive and double tap on it
4. Navigate to D:\FANUC\iHMI\MTB\CNCOpera\Setting
5. Double tap on Setting_Data.txt open with Word Pad (or notepad if you prefer)
6. Scroll down to the following;

[Actual_Feedrate]

Max_Scale-Markings_Val=40000

Change 40000 to 1575

Tap File, Save, and save the file. 

Close out of Word Pad (or Notepad). Close out of Explorer. Navigate back to your CNC screen. You may need to go to another screen to get the display to refresh. Hope that helps. 

 

As to the keyboard not keeping up... I guess I type slower. LOL I did notice the computer doesn't seem to be quite as responsive as a dedicated PC or dedicated CNC. I'm going to do a little more testing between Christmas and New Years and see what I can figure out. 

 

 

Will this work on a robodrill with 31i B5? 

[cncappsjames]

Does it have the iHMI interface and touch panel screen?

[balnh]

Has IHMi interface but not touchscreen. 

[balnh]

Never mind just found it. Navigating without the touchscreen is a pain in the xxxx though. Thanks