[woffler]

Does anyone use V24 with lathe inch post. I have been trying to get one from bobcad for three months now with no luck.
They sent me one but it will not work either so, i am kind of stuck except for the wizards in mach.

[woffler]

I was able to fix Bob's post pro. they had a G95 in there for feed's and you could not turn it off in the software .
I will check further today for threading and other function's to see if they will run OK .

[xj5373]

Hi,
I am trying to get V24 to work with my lathe on Mach 3 and am struggling with post processors. Tried Mach3LathePst and hit a problem with "no S word G96 line 19" - I edited the tool path in Bob to go for a fixed RPM and this seemed to sort that out - I then got a new problem - "F word missing with inverse time arc move line 24"....whatever that means
Have we got a proven post processor for Mach3 that could be shared? I found the older thread on this which didn't seem conclusive. The BobCAD web site has a string of Mach3 turn post porcessors but gives no clues as to which works and indeed why there are more than 1 in the list.
Can Al step in here and help get this sorted??
Thanks
Ian

[aldepoalo]

I would think the standard single line lathe post would work or be a good starting point. I would agree there are many mach 3 posts on the website and god only knows which one is the right one for you, or you or you....

So I am sure we can come up with a solution together. Do you have the single line lathe post? I've attached it. Please post some simple samples and let's get into it.

Also if anyone has a mach lathe post that is known to work, please post it here for us.

[xj5373]

Hi Al,
Thanks for getting back to me on this. I had spoken with support before as the post I had been using was not posting a proper header to get Predator going - The Engine Guy was also very helpful in getting this sorted - you should get him on the payroll along with Burrman!
I attach this post here.
I have continued to work on that little roller thing mentioned in an earlier thread.....it is amazing how much time can get eaten up pursuing these things but it is all part of the learning curve I guess!
Here is the G code (note in radius mode) that BOBCad is generating and Predator is simulating nicely.
Mach is however making a meal of it.....it is as if it is interpreting the arcs "inside out" i.e. rather than follow the path of the bit of the arc BOBCad intends, it goes roun the rest of the circle.
Sure this is a config issue in Bob or the post processor or even Mach - question is which one?
Ian

[xj5373]

Just shooting out for the day - but I just wondered if this is to do with he machinie orientation? BOBCad assumes the tool is coming from the back of the job (where it often is in proper CNC lathes) but in reality the tool on my lathe is coming from the front. Does this mean that CW and ACW are reversed? Should we swap G02 for G03?
When I get back later on I will generate some code using the Mach turning wizard then do the same geometry with BOBCad and compare them - should be revealing.
Ian

[The Engine Guy]

Just shooting out for the day - but I just wondered if this is to do with he machinie orientation? BOBCad assumes the tool is coming from the back of the job (where it often is in proper CNC lathes) but in reality the tool on my lathe is coming from the front. Does this mean that CW and ACW are reversed? Should we swap G02 for G03?
When I get back later on I will generate some code using the Mach turning wizard then do the same geometry with BOBCad and compare them - should be revealing.
Ian

BobCAD assumes the tool is coming from either the old front approach to the material with the toolpost closest to the operator, this also applies to a "standard" slant bed type lathe that approaches the material from the rear but the tool is facing downwards.

This is in effect exactly the same, it is just taking the front toolpost and rotating it around the center line of the lathe so the tool turret/tool post is at the rear.

So, imagine I have an old Lathe with the tool post at the front and using manual tool changing, I wouldn`t change anything from the BobCAD output as BobCAD has already output the code correctly for a rear approach with the tool facing down so that is still correct for my setup.

All the above has the spindle rotating in a standard clockwise direction when viewed from the back of the spindle, not from the chuck, ie M3.

Things only change when you have an "oddball" machine like one of my Lathes, it is a slant bed type with the tool turret at the rear, so far so good, however the turret is setup so the tools are facing upwards which means the spindle has to rotate in the opposite direction ie anti-clockwise so I have to have my Post Processor setup to output an M4 instead of an M3.

One small point, Mach does run in Diameter mode, the numbers on the screen are the diameter of the workpiece so it is entirely possible that it doesn`t like the code arcs you are giving it.

As you can see and from the above and what Al posted there is no "post that works for every one" the post has to be "tweaked" to suit the machine/operator as due to the ability to setup Mach to work differently for different machines/operators.
You haven`t given us much in the way of details of the physical characteristics of your Lathe which makes it difficult to come up with a solution for you
Also if you can upload the BobCAD file you are working on that would be a big help

It looks to me like a combination of setting in Mach and BobCAD Post could be the problem. I`ll have a go at your files when I get a bit more time

Regards

[The Engine Guy]

After running your code through Predator backplot the stock was way to big, double the size required, had you run the code at your machine then it would have crashed

Had a quick "play" with your Post, changed it over to Diameter mode and it seems to be working fine now. Here is the line to change in your Post.

249. Output X as a diameter or radius (d/r)? d

Posting code in Radius mode for Mach3 that is running in Diameter mode isn`t going to work

Regards

[xj5373]

Hi,
Thanks of this. Based on your earlier post I made the "executive decision" to switch to diameter mode. I set this in both Mach and in BOBCad. I then created a simple part and produced G Code in BOBCad and Mach (using a wizard).
I looked at a few things that were puzzling but eventually spotted a Mach parameter under "ports and pins" - "turn options" - it was "reversed arcs in front post". I had this checked for some reason - unchecking it corrects the arcs in Mach, so I now have BOBCad code that looks like it will run on the machine.
I noted that BOBCad is producing G Code with radius terms rather I and K terms like the wizard for G02 aadn G03. I could change this using line 242 in the post but Macc seems happy with either so I will leave it.
I am doing my Mach testing this evening on my laptop in the office - tomorrow I will go live on the machine (Denford Orac).
I still have something a bit odd in Predator where the stock looks too big - I will chase that down tomorrow and work through your mode suggestions.
Thanks again
Ian

[The Engine Guy]

Hi,
Thanks of this. Based on your earlier post I made the "executive decision" to switch to diameter mode. I set this in both Mach and in BOBCad. I then created a simple part and produced G Code in BOBCad and Mach (using a wizard).
I looked at a few things that were puzzling but eventually spotted a Mach parameter under "ports and pins" - "turn options" - it was "reversed arcs in front post". I had this checked for some reason - unchecking it corrects the arcs in Mach, so I now have BOBCad code that looks like it will run on the machine.
I noted that BOBCad is producing G Code with radius terms rather I and K terms like the wizard for G02 aadn G03. I could change this using line 242 in the post but Macc seems happy with either so I will leave it.
I am doing my Mach testing this evening on my laptop in the office - tomorrow I will go live on the machine (Denford Orac).
I still have something a bit odd in Predator where the stock looks too big - I will chase that down tomorrow and work through your mode suggestions.
Thanks again
Ian

Ian

Sounds like you have most of it sorted now, if you haven`t changed the Post line 249 to diameter then the post is outputting the code at half the geometry, so a line you have drawn at 1 inch will be output at 0.5 so Predator will create a full size stock diameter because that isn`t altered by line 249 and then it runs from the G code at half diameter so it starts halfway down the face of the stock.

If you were to run that code in your machine with 1 inch diameter bar stock then the tool would literally try to go into the material at the 0.5 inch point, fairly disasterous consequences I would say

FYI I also have a Denford Orac Lathe But not on Mach3, still on original hardware/software

Do you have the rear tool post for the parting off tool on yours ? ? If so you will need to make some changes to your BobCAD Post and remember to change the tool orientation in BobCAD

Regards

[xj5373]

Ok,
Sticking then with the mode issues then I have converted to use diameter mode exclusively. To do this you need 4 things configured;

Mach3 needs to be set to diameter mode - config - ports and pins - turn options - then check diameter mode. Whilst you are here check that reversed arcs in front post is not checked (unless your machine physical configuration demands it).

BOBCad-CAM needs also to be in diameter mode - preferences - settings part - units - highlight lathe diameter mode

Use a post processor that is also set to diameter mode as described by The Engine Guy - post processor line 249. Output X as a diameter or radius (d-r)? set to d

Finally, if you use predator you need the "machine control emulator" (BOBCad probably have a proper name for this file) to be set to diameter mode. In my case I am using FANUC 16TA. You will find the file by following the path - Predator Software\Common Files\RPost 7.0\Lathe then the file you are using .rpl. Towards the end of this file you will see a line lathe_prog_mode=diameter - ensure that this is diameter and not radius. I think that diameter is the default setting here.

With all these things aligned on diameter mode then it looks like everything is working at least on my PC - Next step is to take the G Code to the machine.
Ian

[xj5373]

Hi,
Moved onto the machine this morning - first thing is M03 to start the spindle is missing in the code - I think this is in section 2 of the post
n,spsp_code,s
This is outputting N04 G97 S1000
I am scratching a bit here - any ideas?

With a manual spindle on - the code seemed to run ok with no work in the machine - put the job in and re-ran the code.......crash!
Not sure what happened, still licking my wounds.
Ian

[SBC Cycle]

Hi,
Moved onto the machine this morning - first thing is M03 to start the spindle is missing in the code - I think this is in section 2 of the post
n,spsp_code,s,spindle_on
This is outputting N04 G97 S1000
I am scratching a bit here - any ideas?

With a manual spindle on - the code seemed to run ok with no work in the machine - put the job in and re-ran the code.......crash!
Not sure what happened, still licking my wounds.
Ian

Maybe? Don't play with the lathe much.

[TonyW]

Hi,
Moved onto the machine this morning - first thing is M03 to start the spindle is missing in the code - I think this is in section 2 of the post
n,spsp_code,s
This is outputting N04 G97 S1000
I am scratching a bit here - any ideas?

With a manual spindle on - the code seemed to run ok with no work in the machine - put the job in and re-ran the code.......crash!
Not sure what happened, still licking my wounds.
Ian

G97 is 'constant rpm' (IE: G97 S1500 M03= 1500 rpm, clockwise rotation)
G96 is Constant surface speed (IE: G96 S500 M03= 500 surface foot, rpm auto calculated by lathe based on the turning diameter, clockwise rotation)

I have attached my very well running post for my Okuma lathe. You can turn debug on in your post, should be line 8. (8. Set debug. debug_off). Just change the debug_off to debug_on. Then when you post your code, it will show you where exactly things are missing. In mine, line 782 and 783 are for spindle forward and reverse. Line #2 gives the command to turn spindle on. (Spindle_on, = on, spindle_off turns it off) That should be in your post as well. In Bobcad, be sure you have either an RPM or Surface foot entered or it will not post an rpm. Try my post with your file and see if it creates the rpm for you.

[The Engine Guy]

Hi,
Moved onto the machine this morning - first thing is M03 to start the spindle is missing in the code - I think this is in section 2 of the post
n,spsp_code,s
This is outputting N04 G97 S1000
I am scratching a bit here - any ideas?

With a manual spindle on - the code seemed to run ok with no work in the machine - put the job in and re-ran the code.......crash!
Not sure what happened, still licking my wounds.
Ian

Ian

Ouch, sounds like you are not having a good day, I must admit I am a little mystified by the machine running the code OK in air and crashing into the material, very odd indeed.

You are sure you didn`t change anything else in the post or the code other than to add the spindle start command ? ?

Did you re-home the machine after the "fresh air" run ? ?
If not and if you are running a G91 (Incremental) command in your first line then if the machine had not been re-homed and it is on incremental then it would start from where it finished on the first run and still move the full amount of the first X and Z coordinate amounts resulting in the pain you felt

Without the BobCAD file and the Mach3 xml file to check the settings I don`t have much else right now I`m afraid.

If you want to PM me I will give you a `phone number you can reach me on if you want to go through anything with me.

P.S. TonyW, Ian has the rpm, just didn`t have the M3

Ian BTW you can just hard code the M3 into the line by putting it in quotes like this:
n, spsp_code,s,"M3"

That is guaranteed to output the M3

Regards

[TonyW]

Yeah, I worded it a little wrong

[The Engine Guy]

Yeah, I worded it a little wrong

At my age I do it all the time, welcome to the "clanger" club

Just been looking at your Okuma Post, doubt it will work with Mach3 as there are things in there that are specific to Okuma in general and your machine setup in particular, but definitely worth the try



$BOBCAD1.NC % (Mach3 is unlikely to regognise this line and will possibly either error out or ignore it, might need removing)
N0 G140 (Specific to your Okuma for main spindle, again Mach3 may not recognise it, might need removing)
( PROGRAM NAME: BOBCAD1.NC)
( PROGRAM START - TURNING CYCLES )
( POST: Okuma_OSPU100L )
(TUE. 08/07/201207:20PM)
G50 S2000
M42 (Not required, only single speed drive train, again it may skip this or error out, might need removing)
G00 X20 Z20 (As this is hard coded into the Post it will always output, Ians Lathe doesn`t have that much travel, big crash if it travels 20 inches towards the chuck, this would have to go )
N1 (TOOL #1 80 DEG. 1/64 ROUGH TURNING)

End of code :-

Z5.
V40=V40+1 (This looks to be specific to Okuma, think Mach3 would definitely error out on this one)
M30
%

Mach3 would expect something like this:

Z5.
M5
M9
M30
%

A good basic Fanuc Post with just a few "tweaks" should be OK for Mach3, this control software is pretty much designed around the basic Fanuc coding.

Regards

[aldepoalo]

These are samples from the single line post:




free image hosting




With canned cycles:

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(LTOOL T0202 M0200 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
 
O0001
(JOB 1  ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
N1 G80 G93 G40 G99 G18 G20 G90
N2 T0101 M06
N3 M40
N4 G50 S500
N5 G96 S500 M03
N6 M08
N7 G00 X2. Z.05
N8 G71 P9 Q12 U.02 W.02 D.03 F5.
N9 G00 X0.
N10 G01 Z-.25
N11 G01 X1.5
N12 G01 Z-2.
N13 G40
N14 M01
N15 M09
N16 G00 X4. Z.05
N17 G00 Z1.
(TOOL #2 80 DEG. 1/64 FINISH TURNING )
N18 T0202 M06
N19 M40
N20 G50 S500
N21 G96 S200 M03
N22 M08
N23 G00 X2. Z.05
N24 G70 P9 Q12 F.015
N25 G97
N26 G40
N27 M01
N28 G00 X4.
N29 G00 Z1.
N30 M05
N31 M30

With separate moves :

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(LTOOL T0202 M0200 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
 
O0001
(JOB 1  ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
N1 G80 G93 G40 G99 G18 G20 G90
N2 T0101 M06
N3 M40
N4 G50 S500
N5 G96 S500 M03
N6 M08
N7 G00 X2.2 Z.07
N8 G00 X1.94
N9 G01 Z-2. F5.
N10 G00 X2.
N11 G00 Z.07
N12 G00 X1.88
N13 G01 Z-2.
N14 G00 X1.94
N15 G00 Z.07
N16 G00 X1.82
N17 G01 Z-2.
N18 G00 X1.88
N19 G00 Z.07
N20 G00 X1.76
N21 G01 Z-2.
N22 G00 X1.82
N23 G00 Z.07
N24 G00 X1.7
N25 G01 Z-2.
N26 G00 X1.76
N27 G00 Z.07
N28 G00 X1.64
N29 G01 Z-2.
N30 G00 X1.7
N31 G00 Z.07
N32 G00 X1.58
N33 G01 Z-2.
N34 G00 X1.64
N35 G00 Z.07
N36 G00 X1.52
N37 G01 Z-.25
N38 G01 Z-2.
N39 G00 Z.07
N40 G00 X1.46
N41 G01 Z-.23
N42 G01 X1.4707
N43 G03 X1.4821 Z-.2302 I.0016 K-.0338
N44 G01 X1.4954 Z-.2315
N45 G01 X1.5063 Z-.2352
N46 G03 X1.51 Z-.2372 I-.0016 K-.0034
N47 G01 X1.5166 Z-.2421
N48 G01 X1.518 Z-.2451
N49 G01 X1.52 Z-.25
N50 G00 Z.07
N51 G00 X1.4
N52 G01 Z-.23
N53 G01 X1.46
N54 G00 Z.07
N55 G00 X1.34
N56 G01 Z-.23
N57 G01 X1.4
N58 G00 Z.07
N59 G00 X1.28
N60 G01 Z-.23
N61 G01 X1.34
N62 G00 Z.07
N63 G00 X1.22
N64 G01 Z-.23
N65 G01 X1.28
N66 G00 Z.07
N67 G00 X1.16
N68 G01 Z-.23
N69 G01 X1.22
N70 G00 Z.07
N71 G00 X1.1
N72 G01 Z-.23
N73 G01 X1.16
N74 G00 Z.07
N75 G00 X1.04
N76 G01 Z-.23
N77 G01 X1.1
N78 G00 Z.07
N79 G00 X.98
N80 G01 Z-.23
N81 G01 X1.04
N82 G00 Z.07
N83 G00 X.92
N84 G01 Z-.23
N85 G01 X.98
N86 G00 Z.07
N87 G00 X.86
N88 G01 Z-.23
N89 G01 X.92
N90 G00 Z.07
N91 G00 X.8
N92 G01 Z-.23
N93 G01 X.86
N94 G00 Z.07
N95 G00 X.74
N96 G01 Z-.23
N97 G01 X.8
N98 G00 Z.07
N99 G00 X.68
N100 G01 Z-.23
N101 G01 X.74
N102 G00 Z.07
N103 G00 X.62
N104 G01 Z-.23
N105 G01 X.68
N106 G00 Z.07
N107 G00 X.56
N108 G01 Z-.23
N109 G01 X.62
N110 G00 Z.07
N111 G00 X.5
N112 G01 Z-.23
N113 G01 X.56
N114 G00 Z.07
N115 G00 X.44
N116 G01 Z-.23
N117 G01 X.5
N118 G00 Z.07
N119 G00 X.38
N120 G01 Z-.23
N121 G01 X.44
N122 G00 Z.07
N123 G00 X.32
N124 G01 Z-.23
N125 G01 X.38
N126 G00 Z.07
N127 G00 X.26
N128 G01 Z-.23
N129 G01 X.32
N130 G00 Z.07
N131 G00 X.2
N132 G01 Z-.23
N133 G01 X.26
N134 G00 Z.07
N135 G00 X.14
N136 G01 Z-.23
N137 G01 X.2
N138 G00 Z.07
N139 G00 X.08
N140 G01 Z-.23
N141 G01 X.14
N142 G00 Z.07
N143 G00 X.02
N144 G01 Z-.23
N145 G01 X.08
N146 G00 X0.
N147 G01 X.02
N148 G00 X4.
N149 G00 Z1.
N150 G40
N151 M01
N152 M09
(TOOL #2 80 DEG. 1/64 FINISH TURNING )
N153 T0202 M06
N154 M40
N155 G50 S500
N156 G96 S200 M03
N157 M08
N158 G00 X2.2 Z.05
N159 G00 X0.
N160 G01 Z-.25 F.015
N161 G01 X1.5
N162 G01 Z-2.
N163 G00 X4.
N164 G00 Z1.
N165 G40
N166 M01
N167 M09
N168 M05
N169 M30

The single line lathe post would be a generic Fanuc style that I would think would be very close to what mach 3 might want.

[xj5373]

Hi All,
Thanks for helping out on this - I am going to be absent for a few days now as I have an appointment at the Olympics - I am not competing you understand, although I will pack my gym kit and pumps in case they need a hand!
I will be back to this next week.
Thanks to Rob for the offer of some hand holding - I will almost certainly give you a call once I am back.
Ian

[xj5373]

P.S. TonyW, Ian has the rpm, just didn`t have the M3

Ian BTW you can just hard code the M3 into the line by putting it in quotes like this:
n, spsp_code,s,"M3"

That is guaranteed to output the M3

Found by comparing my post with Al's (which gives a Mach 3 error - F word missing with inverse time g1 move .....whatever that means?) that if you change the line to
n, spsp_code,s,spindle_on
you get the M03.

Comparing the different posts my impresion is that they are edited to death one way or another - there are so many differences between posts it is hard to work out what is doing what.

Al - Is there any kind of a document that would help me get under the skin of how the post works?

Ian