I widened the indexing slot to 12mm. This improved the reading a bit. 500 +-3 RPM. But it didn't solve my problem. Program still waits at that line.
Mactec I'll try your code today.
Sent from my MI 5s Plus using Tapatalk
Um ... are you using Mach3?
D parameter: not used in Mach3
F parameter: not used in Mach3 in this command
Why X8.16 instead of X8.2?
Why P1? The OP wants P1.5
And I don't understand the double G76 command.
Help!
Cheers
Roger
I widened the indexing slot to 12mm. This improved the reading a bit. 500 +-3 RPM. But it didn't solve my problem. Program still waits at that line.
Mactec I'll try your code today.
Sent from my MI 5s Plus using Tapatalk
Suat
Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby
The X8.16 was what the software gave for the 10 x 1.5 thread using a 10mm dia
It can be done both ways 2 lines is more common, in the real world, a single line works also if formatted correctly
Mach3 pretty much runs anything you throw at it, unless it is formatted in such a way that it does not know what to do
Mactec54
I think I've found another problem. I measured the input voltage of the C3 indexing board and it was 3.5 volt. And the output is even lower. It must be 5v. Maybe this is the reason for the bad RPM reading.
I have a 5v power supply in the cabinet and I use it for both BB and C3. Now I need a dedicated power supply for the C3.
Sent from my MI 5s Plus using Tapatalk
Suat
Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby
Hi Mactec
G76 P010060 Q0.020 R0.0200
G76 X8.160 Z-10.000 P0.920 Q0.300 F1.500 R0.000 P1
Sorry, but this code will not even load into Mach3. I tried.
Line 1:
P010060: a pitch of 10,060 mm - really?
R0.0200: an X start value - less than the pitch
Q0.020: the number of spring passes - should be integer, and probably >=1
Line 2:
P0.920: pitch - OK but not 1.5 mm as wanted
Q0.300: spring passes
F1.500: invalid in G76 instruction
R0.000: X start of zero?
O1: parameter repeated - invalid
I suspect this code is for something other than Mach3: it cannot run under Mach3.
Cheers
Mactec54
Hi Mactec
Sorry, but it won't even LOAD into Mach3. I tried.
I have been through the Fanuc manual and I don't think it is the same as the NIST-Standard Mach3 language. Many instructions are the same, but not all. The example you show is NOT from the Mach3 manual. Maybe the Mach4 manual?
It is no use quoting the Mach4 guide- we know that it is a bit different - closer to Fanuc. Different animal.
Now, why did Artsoft decide to make the Mach4 language incompatible with Mach3 and NIST? I don't know, but perhaps they decided to head in the Fanuc direction, to garner market share? Regardless of why, that does place a huge barrier to the adoption of Mach4 over Mach3. Personally, I think it was a mistake, but I am biased.
EDIT:
So I went for a wander through the web. Yes, the strange G76 code comes from the Fanuc manual. It is totally incompatible with Mach3 and NIST.
More of a worry: there seem to be different versions of the Fanuc G-code - different generations. And the Fanuc g-code for a mill is different from that for a lathe. On a mill, G76 is for boring a hole.
That means that while a Mach3 program can be run on any machine using Mach3, a Fanuc program is NOT portable even between different Fanuc controllers, and not between different machine brands. Oh well.
Cheers
Roger
Last edited by RCaffin; 10-22-2017 at 07:43 PM.
Do you have Mach3 Lathe program running, it won't run if you, just have the Mill program, Mach3 lathe is totally different, this runs on Mach3 I just ran it, here is another Fanuc program also runs on Mach3, Mach4 programing is just the same go through the PDF I posted, they use the same format, I have just tried 4 different formats, 2 not being Fanuc and they all will run on Mach3
%
O2001
( FANUC , SYSTEM UNIT 1 MM )
( EXTERNAL THREAD, RH, TOWARDS THE CHUCK)
( THREAD DIA = 10.000 , PITCH 1.5 MM , LENGTH = 10.000)
( START THREAD PLAN . Z=0 )
( TOOLHOLDER = SER 12 12 K11 )
( INSERT = 11 ER A60 )
G50 S2000
G28 U0 W0
T0202 G99 G97 M03 S318
G00 X14.685 Z11.954 M08
G00 Z0.954
G76 P010060 Q20 R0.0200
G76 X8.160 Z-10.000 P920 Q300 F1.500 R0.000
G28 U0 W0
M30
%
Just tried the Mach3 wizard, if that is what you are using it works fine, they have done a good job with that, I loaded the program above, it runs but does not machine the thread correctly so stick with what works for the Mach3 control software
Last edited by mactec54; 10-23-2017 at 09:07 AM. Reason: changed post
Mactec54
Mactec54
Hi Mactec
Yes, I run a mill using Mach3 for mill, and a lathe using Mach3 for lathe. I have been using both for several years in a semi-production mode. And i do quite a lot of threading on the lathe.
G76 X8.160 Z-10.000 P920 Q300 F1.500 R0.000
This tells My Mach3Turn that the Pitch is 920 mm, there are 300 spring passes, and since R, which is Xstart, is <Xend of 8.16, it does an internal threading. I suspect it simply ignores the F1.50.
Yes, this did 'run' once I took thesecond P1 off the line. But what it tried to do was ... strange.
The code may run quite happily on a Fanuc controller, because the Fanuc G76 instruction is totally different from the Mach3 instruction. So the parameters all have different meanings. For example, R is the X start value in NISTland but it is the taper in FanucLand. Q is the cut volume in FanucLand, but it is the number of spring passes in NISTland.
In addition, Fanuc parameters for G76 are in microns, while Mach3 and NIST use millimetres or inches. So P920 means 0.92 mm in FanucLand and 920 mm in NISTland. The same applies to Q, both meaning and units.
Cheers
Roger
I will dispute the 'not the norm' claim. Mach3 follows NIST very closely. Fanuc varies between Fanuc versions, but does NOT follow NIST. Other controllers are different again.
Me, I am biased, thinking that the NIST version is 'the norm' today. It is followed by most or all of the current generation of PC controllers.
Cheers
Roger
That is correct if you know what the differences are like the P and the Q you just change them, when I loaded the last program Mach3 told me the Tool Radius was to large, so you just change that and you run
Check Mach4 they are using the same as what I have been showing, they have moved / changed everything to be more compliant industry standards
We have been through this before the Code standards are all compliant with the RS 274 and ISO standards
Mactec54
Hi again,
I have a question. Can I connect a hall effect sensor directly to an input on the BB? If yes, is it best feeding the sensor with a 5v external power supply? Or take the 5v from the BB?
Suat
Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby
This video may help with your index pulse
https://www.youtube.com/watch?time_c...&v=D6FzmJ5vpgs
Mactec54
Hi again.
I tried everything without luck. At last I changed the computer with a newer one and did the same calibration. The RPM seem to be very stable now. The curve isn't as it should be but at least I've completed the calibration. I think I'm in a point where I can do fine tuning, finally.
Sent from my MI 5s Plus using Tapatalk
Suat
Proud father, C# developer, Model heli pilot, newbie free time machinist for hobby