[aldepoalo]

For those of you that do not understand how to edit a post processor this video should give you some basic concepts.

[ferrumdg]

So now let's look at shifted holes.


1) You did not pick your part origin correctly
2) When you setup Zero on the machine it was off slightly.


Let's look at first possibility. When choosing your part origin in BobCAD either when running the stock wizard, or after when you edit your machine setup and edit your origin. When you go into selection mode for your origin "snaps" are turned on. When you click on a point it picks up that snap location, right all well and good. One "snaps" that is turned on that can be problematic is "screen position" Now I am not sure why you would want to "sketch" a origin, but because it's , it's possible. So maybe what is happens some times is you think you picked a point, but really you picked a screen posting that is very close to the point you wanted for your origin.

Let's look at the second possibility, this one could be your hiccup, depending on setup and work flow. I can't say this is where you are going wrong, but if you holes / geometry are shifted the defined zero on the machine could be the issue.

If you can show me a part program and g-code program where the hole drawing locations and posted codes do not match I can help you further on this issue. Otherwise I have to chalk this up to user error somewhere... I don't say that to offend you, it's just the most likely reason why you are having this problem.

Al,

Assuming I'd set the wrong Zero on the MACHINE - then EVERYTHING should be at an offset - shouldn't it?
At least according to my logic.

Now this is the reality I'm talking about though:
Attachment 266690
The hole row at which I'm pointing the pen is as it is supposed to be...
The upper row is what happened when I ran the programm the first time!

Now I chose to post ONLY the drill feature in a separate file - and without ANY change to the machine side or to the settings in BobCAD I ran the individual file again on the same part (the part was ruined anyhow, so I didn't care).
I did not change Zero, I didn't move the stock, I didn't change ANYTHING AT ALL, aside from re-posting only the drill feature to a new file and ran this.
When I did this, the holes were indeed made in the CORRECT position.


mind you that the first feature (originally the program only had two features, the basic pockets and the holes) the pockets were placed perfectly...

I really do not understand why this happens.
Especially as it's an on / off thing. but EVERY time it happend it was with a drilling thing - never with anything else.

[aldepoalo]

I am not sure what happened, all I can look at on my end is your drawing and code. So I checked the hole locations on your drawing against the hole locations posted in your code. They matched, so it's really hard to say why the locations where shifted when your ran them on the machine.

These are the locations I pulled off your drawing.

Hole 1 X10.091 Y -6.68
Hole 2 X6.949 Y-50.604
hole 3 X4.182 Y-95.009

These are the hole locations in the g-code

N430 X10.091 Y-6.680
N455 X6.949 Y-50.604
N479 X4.182 Y-95.009

[aldepoalo]

Holes posted by themselves:

%100
N0001 ( P: MARCEL_OUTDOOR1.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 11:35AM)
N0005 G90 G80 G71 G40 G17
N0006 (JOB 2  HOLE  RANDOM POINT PATTERN)
N0007 (FEATURE DRILL HOLE)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.17 M06
N0013G43
N0014 S6000 M03
N0015 G54
N0016 G00 G90 X-10.091 Y6.68 Z2.54 <<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0017 M08
N0018 G01 Z1.88 F120.
N0019 G00 Z2.54
N0020 Z4.42
N0021 G01 Z0.23
N0022 G00 Z2.54
N0023 Z2.77
N0024 G01 Z-1.42
N0025 G00 Z2.54
N0026 Z1.12
N0027 G01 Z-3.07
N0028 G00 Z2.54
N0029 Z-0.53
N0030 G01 Z-4.72
N0031 G00 Z2.54
N0032 Z-2.18
N0033 G01 Z-6.37
N0034 G00 Z2.54
N0035 Z-3.83
N0036 G01 Z-8.02
N0037 G00 Z2.54
N0038 Z-5.48
N0039 G01 Z-8.261
N0040 G00 Z2.54
N0041 X-6.949 Y50.604 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0042 G01 Z1.88
N0043 G00 Z2.54
N0044 Z4.42
N0045 G01 Z0.23
N0046 G00 Z2.54
N0047 Z2.77
N0048 G01 Z-1.42
N0049 G00 Z2.54
N0050 Z1.12
N0051 G01 Z-3.07
N0052 G00 Z2.54
N0053 Z-0.53
N0054 G01 Z-4.72
N0055 G00 Z2.54
N0056 Z-2.18
N0057 G01 Z-6.37
N0058 G00 Z2.54
N0059 Z-3.83
N0060 G01 Z-8.02
N0061 G00 Z2.54
N0062 Z-5.48
N0063 G01 Z-8.261
N0064 G00 Z2.54
N0065 X-4.182 Y95.009 <<<<<<<<<<<<<<<<<<<<<<<<
N0066 G01 Z1.88
N0067 G00 Z2.54
N0068 Z4.42
N0069 G01 Z0.23
N0070 G00 Z2.54
N0071 Z2.77
N0072 G01 Z-1.42
N0073 G00 Z2.54
N0074 Z1.12
N0075 G01 Z-3.07
N0076 G00 Z2.54
N0077 Z-0.53
N0078 G01 Z-4.72
N0079 G00 Z2.54
N0080 Z-2.18
N0081 G01 Z-6.37
N0082 G00 Z2.54
N0083 Z-3.83
N0084 G01 Z-8.02
N0085 G00 Z2.54
N0086 Z-5.48
N0087 G01 Z-8.261
N0088 G00 Z2.54
N0089 M09
N0090 M05
N0091 G74 Z X
N0092 M30

Holes posted with other ops after :

%100
N0001 ( P: MARCEL_OUTDOOR1.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 11:37AM)
N0005 G90 G80 G71 G40 G17
N0006 (JOB 2  HOLE  RANDOM POINT PATTERN)
N0007 (FEATURE DRILL HOLE)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.17 M06
N0013G43
N0014 S6000 M03
N0015 G54
N0016 G00 G90 X-10.091 Y6.68 Z2.54  <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0017 M08
N0018 G01 Z1.88 F120.
N0019 G00 Z2.54
N0020 Z4.42
N0021 G01 Z0.23
N0022 G00 Z2.54
N0023 Z2.77
N0024 G01 Z-1.42
N0025 G00 Z2.54
N0026 Z1.12
N0027 G01 Z-3.07
N0028 G00 Z2.54
N0029 Z-0.53
N0030 G01 Z-4.72
N0031 G00 Z2.54
N0032 Z-2.18
N0033 G01 Z-6.37
N0034 G00 Z2.54
N0035 Z-3.83
N0036 G01 Z-8.02
N0037 G00 Z2.54
N0038 Z-5.48
N0039 G01 Z-8.261
N0040 G00 Z2.54
N0041 X-6.949 Y50.604 <<<<<<<<<<<<<<<<<<<<<<
N0042 G01 Z1.88
N0043 G00 Z2.54
N0044 Z4.42
N0045 G01 Z0.23
N0046 G00 Z2.54
N0047 Z2.77
N0048 G01 Z-1.42
N0049 G00 Z2.54
N0050 Z1.12
N0051 G01 Z-3.07
N0052 G00 Z2.54
N0053 Z-0.53
N0054 G01 Z-4.72
N0055 G00 Z2.54
N0056 Z-2.18
N0057 G01 Z-6.37
N0058 G00 Z2.54
N0059 Z-3.83
N0060 G01 Z-8.02
N0061 G00 Z2.54
N0062 Z-5.48
N0063 G01 Z-8.261
N0064 G00 Z2.54
N0065 X-4.182 Y95.009 <<<<<<<<<<<<<<<<<<<<<
N0066 G01 Z1.88
N0067 G00 Z2.54
N0068 Z4.42
N0069 G01 Z0.23
N0070 G00 Z2.54
N0071 Z2.77
N0072 G01 Z-1.42
N0073 G00 Z2.54
N0074 Z1.12
N0075 G01 Z-3.07
N0076 G00 Z2.54
N0077 Z-0.53
N0078 G01 Z-4.72
N0079 G00 Z2.54
N0080 Z-2.18
N0081 G01 Z-6.37
N0082 G00 Z2.54
N0083 Z-3.83
N0084 G01 Z-8.02
N0085 G00 Z2.54
N0086 Z-5.48
N0087 G01 Z-8.261
N0088 G00 Z2.54
N0089 M09
N0090 M05
(JOB 3  PROFILE)
(FEATURE PROFILE)
N0091 ( TOOL CHANGE )
N0092 M05
N0093 G74 Z X
N0094 T00.12 M06
N0095G43
N0096 S6000 M03
N0097 G54
N0098 G90
N0099 X-3.08 Y112.671
N0100 M08
N0101 Z2.54
N0102 G00

Holes with ops before:

N0413 G01 Z-4. F 75.
N0414 X-5.741 Y-0.162 Z-4.314
N0415 X-8.718 Y0.214 Z-4.735
N0416 X-5.741 Y-0.162 Z-5.157
N0417 X-8.718 Y0.214 Z-5.578
N0418 X-5.741 Y-0.162 Z-6.
N0419 X-12.707 Y0.717 F260.
N0420 X-10.054 Y-5.739
N0421 X-5.912 Y-1.585
N0422 G02 X-5.741 Y-0.162 R614.696
N0423 G00 Z2.54
N0424 M09
N0425 M05
(JOB 2  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)
N0426 ( TOOL CHANGE )
N0427 M05
N0428 G74 Z X
N0429 T00.17 M06
N0430G43
N0431 S6000 M03
N0432 G54
N0433 G90
N0434 X-10.091 Y6.68 <<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0435 M08
N0436 Z2.54
N0437 G01 Z1.88 F120.
N0438 G00 Z2.54
N0439 Z4.42
N0440 G01 Z0.23
N0441 G00 Z2.54
N0442 Z2.77
N0443 G01 Z-1.42
N0444 G00 Z2.54
N0445 Z1.12
N0446 G01 Z-3.07
N0447 G00 Z2.54
N0448 Z-0.53
N0449 G01 Z-4.72
N0450 G00 Z2.54
N0451 Z-2.18
N0452 G01 Z-6.37
N0453 G00 Z2.54
N0454 Z-3.83
N0455 G01 Z-8.02
N0456 G00 Z2.54
N0457 Z-5.48
N0458 G01 Z-8.261
N0459 G00 Z2.54
N0460 X-6.949 Y50.604 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0461 G01 Z1.88
N0462 G00 Z2.54
N0463 Z4.42
N0464 G01 Z0.23
N0465 G00 Z2.54
N0466 Z2.77
N0467 G01 Z-1.42
N0468 G00 Z2.54
N0469 Z1.12
N0470 G01 Z-3.07
N0471 G00 Z2.54
N0472 Z-0.53
N0473 G01 Z-4.72
N0474 G00 Z2.54
N0475 Z-2.18
N0476 G01 Z-6.37
N0477 G00 Z2.54
N0478 Z-3.83
N0479 G01 Z-8.02
N0480 G00 Z2.54
N0481 Z-5.48
N0482 G01 Z-8.261
N0483 G00 Z2.54
N0484 X-4.182 Y95.009 <<<<<<<<<<<<<<<<<<<<<<<<<<<<
N0485 G01 Z1.88
N0486 G00 Z2.54
N0487 Z4.42
N0488 G01 Z0.23
N0489 G00 Z2.54
N0490 Z2.77
N0491 G01 Z-1.42
N0492 G00 Z2.54
N0493 Z1.12
N0494 G01 Z-3.07
N0495 G00 Z2.54
N0496 Z-0.53
N0497 G01 Z-4.72
N0498 G00 Z2.54
N0499 Z-2.18
N0500 G01 Z-6.37
N0501 G00 Z2.54
N0502 Z-3.83
N0503 G01 Z-8.02
N0504 G00 Z2.54
N0505 Z-5.48
N0506 G01 Z-8.261
N0507 G00 Z2.54
N0508 M09
N0509 M05
N0510 G74 Z X
N0511 M30

I just don't see the shift in the code. Not in the programs I am creating on my side, or the program you sent me that you used when the shift occurred. I do not see the shift in the code. If I did see a shift in the code that would be one thing, but I don't the code post the same hole locations no matter if they are posted by themselves, pre ops or post ops....

hmmm what could it be ..... Does the machine use work offsets like G54 G55? I don't see any in your program.. I really want to help you with this, I just can't see the shift in the code we are creating.

[ferrumdg]

Holes posted by themselves:



I just don't see the shift in the code. Not in the programs I am creating on my side, or the program you sent me that you used when the shift occurred. I do not see the shift in the code. If I did see a shift in the code that would be one thing, but I don't the code post the same hole locations no matter if they are posted by themselves, pre ops or post ops....

hmmm what could it be ..... Does the machine use work offsets like G54 G55? I don't see any in your program.. I really want to help you with this, I just can't see the shift in the code we are creating.

This is so weird....

I'll check the files again I have on storage...

About Work Offsets: yes & no.
Yes - the machine does support / have work offsets, but I rarely use them as most of the work I use the machine's Zero as a starting point (homing the all axis') and then use an 3D Probe to actually set Zero on the individual part.
The reason why I mostly do this like that is because I use a great number of individual fixtures, etc.... so basically I'd be reprogramming the machine's offset all the time and I figured it doesn't make too much sense.

Or is there any error in that approach?


About the problem - I doubt it has to do with the actual coordinates... it must correlate with the other issues - all surrounding / being caused by drill operations.
There's the other Issue I had described: Center Drill - followed by drill resulting in code that my machine can't run as it wants to call some sub-routine that simply doesn't exist, completely aside from the fact that I can never see where exactly in the code a sub would be called.
Post it separately - and it works.

I guess some other parameter / command issued by the drilling cycle is somehow "misinterpreted" by the controller and causing all sort of gremlin-****.
if that makes any sense.

btw. did you get my e-mail?

[aldepoalo]

"work I use the machine's Zero as a starting point (homing the all axis') and then use an 3D Probe to actually set Zero on the individual part"

Between runs did you re home the machine? How does you machine pick up home, limit switches?

[aldepoalo]

ferrumdg,

I would love to say, look here in the code see that's where the problem is... But that is not the case. If it were it would be easy to sort you out and have you moving forward. What we have found is 2 problems with your post.

Rapid Z move at tool change to clearance

The need to update your drill cycles to the proper canned cycle format ( as listed in this thread )
Or to put all cycles in separate moves to eliminate and canned cycle format issues


As far as the shift in the program, that's not something that is happening in the code ( IMO ) I do not see anything in the code that points to the shift. Posting drilling with pre or post ops was not the problem either as far as I can tell. I have the.pim file you ran when this shift issue happened. The drill cycle is a pecking cycle which is done with separate moves so no canned cycle issue there. The hole locations are the same no matter what way you post them. ( in the g code ) .

The only thing I can think of is some kind of offset issue at the control based on machine zero or part zero that you setup up....

Like you said it's random and your not sure how to recreate the issue. I am going to call fagor and see what they have to say about it, maybe they'll have some insight...

[ferrumdg]

"work I use the machine's Zero as a starting point (homing the all axis') and then use an 3D Probe to actually set Zero on the individual part"

Between runs did you re home the machine? How does you machine pick up home, limit switches?

basically the servos are indexed.

I'm no expert on how those things work...
but it has both - limit switches (overrun protection) and index.
from what I gather it uses the indexer for homing.

But the problem is - the machine is old and the company who makes it isn't around anymore.
It was a smaller swiss company building the mill for the watch making industry.

I didn't get any proper documentation or anything like that.
so it's a tad difficult to be certain.


However it certainly is not an issue of the machine I guess...
why? - because all other operations work as they should... before and after.

Don't get me wrong - if you think I'm using the wrong approach, by all means - let me know...
I'm all in favor of constructive criticism.

[aldepoalo]

If it's an issue with the code, there will be a clear culprit , What throws me off is you say if you run the just the drilling op it works. the drilling code by it self or in a group of ops pre or post, the hole locations are the same.. The code is posted in absolute , so if the hole location is correct, then it's correct... Very strange, I am still leaning to some offset issue on the controller.

[ferrumdg]

If it's an issue with the code, there will be a clear culprit , What throws me off is you say if you run the just the drilling op it works. the drilling code by it self or in a group of ops pre or post, the hole locations are the same.. The code is posted in absolute , so if the hole location is correct, then it's correct... Very strange, I am still leaning to some offset issue on the controller.

Al,

So far on two fronts: good news:

the suggested modifications to the post you've made have successfully solved the other two problems!

Rapid Z works now flawlessly and so does the drilling / center drilling / etc. no more errors.
Thanks!

The question I still have though is that looking at the Post, there's numerous other parts that feature the "N1" thing at the end...
I didn't put that there and I have no clue what it should do in the first place - but obviously it's a source for a problem.
What should I do about the rest?
What about all the other things? fast peck, tapping? do I need sub-routines like the one you did supply for the drilling?
I'd much appreciate if you'd show me what else I have to change to the post not to run into these issues again on another project.



Now about the offset issue?
You mention "offset issue on the controller".
From your experiences - how can that happen if the rest works as it should?
The only times I ran into it were always in connection with a drilling operation... can that old POST with that "N1" thing have caused some confusion to the controller??
Or anything like that?

Also based on your (or anyone else' here) experience - is it problematic using the absolut coords as I do in general?
I've got a long number of years worth of experience in conventional / manual machining, but the CNC world is something I basically am still a "beginner" of sorts.
So I do indeed appreciate any kind of feedback that helps to solve operational mistakes on my end.


Thanks.

[aldepoalo]

The question I still have though is that looking at the Post, there's numerous other parts that feature the "N1" thing at the end...
I didn't put that there and I have no clue what it should do in the first place - but obviously it's a source for a problem.
What should I do about the rest?
What about all the other things? fast peck, tapping? do I need sub-routines like the one you did supply for the drilling?
I'd much appreciate if you'd show me what else I have to change to the post not to run into these issues again on another project.


Very good point, the 2 drill cycles that are know to work at this point would be the G81 and G83 blocks. The rest of the drill cycles that have the "N1" I will assume that they do not work correctly. You would need to test to see if there are any problems. The G84 would be the tapping cycle and I am not sure if you are using floating or rigid. Either way you should assume unless tested and know to work that the other cycles do not work correctly.

So the question is are you going to use fast peck, or tapping, if so you need to create a test program, verify they work or not. If they don't work, then fix them ( with help ) if they do work, then use them. This really is the case for any post, until you have tested programs and know that drilling etc are working assume they are not...

As far as no offset or some other shift in the code, it could happen based on modes the controller offers, Usually the controller will display what mode it's in. Really the best thing I can recommend is to read through your manual to learn more about the options and settings your controller has.

How could an offset effect 1 part of the program and not the other. Well tools have offsets in Z and in X& Y, So an offset for a tool that is called could effect just those ops that tool is used in. When the tool changes a new offset is loaded....

The G43 is a length offset and each tool uses one. This is why after you zero your tool in z when you call it, it goes to the right z depth. Each tool typically has it's own G43 value because most tools have different lengths.

G41 /G42 cutter com, this effects an X Y posting for the cutter

G54 work offsets
G92.1 posting move
Etc...

There are different codes that the control can use to offset what is programmed vs where the tool goes. Now I didn't see any offsets like G41 in your code, and if I re look through your code I see consistent posting. Or in other words the code at tool changes , start and end are the same no matter if posted by it self or in a group of ops. So nothing caught my eye as what could be causing the issue. Again I am not sure what caused the shift and like you said it doesn't happen all the time. So if you can't reproduce consistently it's really hard to trouble shoot.



As far as programming ABS or INC, well it can go either way. Pros and cons both ways. I recommend to stay in ABS at this time, this way what you are reading on the DRO are relative to your origin. So in other works you can easy see where things are and where they are going. I am sure other may chip in on abs vs inc, but that is what I recommend at this time.

[ferrumdg]

The question I still have though is that looking at the Post, there's numerous other parts that feature the "N1" thing at the end...
I didn't put that there and I have no clue what it should do in the first place - but obviously it's a source for a problem.
What should I do about the rest?
What about all the other things? fast peck, tapping? do I need sub-routines like the one you did supply for the drilling?
I'd much appreciate if you'd show me what else I have to change to the post not to run into these issues again on another project.


Very good point, the 2 drill cycles that are know to work at this point would be the G81 and G83 blocks. The rest of the drill cycles that have the "N1" I will assume that they do not work correctly. You would need to test to see if there are any problems. The G84 would be the tapping cycle and I am not sure if you are using floating or rigid. Either way you should assume unless tested and know to work that the other cycles do not work correctly.

So the question is are you going to use fast peck, or tapping, if so you need to create a test program, verify they work or not. If they don't work, then fix them ( with help ) if they do work, then use them. This really is the case for any post, until you have tested programs and know that drilling etc are working assume they are not... .

I use Fast pecking quite a lot - and ran into similar issues as with the standard drill and pecking.

I have not much used tapping so far for a multitude of reasons - one being that I have only a limited selection of floating tap holders and rigid tapping is - as far as I understand - only really possible if the machine does spindle indexing, which mine doesn't.
So rigid has been out of the question... and those floating tap holders aren't exactly cheap or easy to come by especially for SK30 DIN 2080... so I have like two and that's it.


So certainly:
- Fast Pecking (is this the one in the post with the No. 73? "High Speed Peck"??)
- Boring
- Tapping

The Subroutine you did add for the Pecking - (2002) - I guess I'd need one of these as well for the fast pecking? how about the rest?


Al - The point for me here is this... I need this working, and from what I understand one working post processor is included with my BobCAD-CAM Purchase.
Clearly the post I have is not finalized up to the task.
Don't get this the wrong way - I do appreciate your help here A LOT! ....
But frankly, I'd like BobCAD to send me the modified post with those functions working.
Obviously, as I had just tested - the modified functions you have provided work as they should.
As to this day I have not gotten a fully functional Post and already had to do a lot of changes myself and figure things out myself I would really appreciate if - as was the deal - I would finally get one working post.
Now you have provided another partial improvement (thanks again) - but ask me to basically do the rest of the work myself. I don't really think that this was what was intended with "one working post".


The Issue with the shifted holes: I can agree that this is tricky to trouble shoot - too many unknown variables.
But let us set that aside for the moment and concentrate on the working post.
Maybe if all that is solved the other problem is solved too?
Or at least I have removed a few of the unknowns from the equation and will be able to investigate this issue further.

[aldepoalo]

- Fast Pecking (is this the one in the post with the No. 73? "High Speed Peck"??)
- Boring
- Tapping


We have an option in the post to tell it to use canned cycle or use separate moves. So for the fast peck if you need it and you do not know the format of the canned cycle then we can just turn separate moves on.

These are the block in your post that affect drill cycles as canned or separate moves.

230. Use Standard drilling canned cycle? y
231. Use peck drill canned cycle? n
232. Use High speed peck drill canned cycle? n
233. Use tapping canned cycle? y
234. Use boring cycle #1 canned cycle? y
235. Use boring cycle #2 canned cycle? y
236. Use back boring cycle canned cycle? n
237. Use left hand tap cycle canned cycle? n
238. Use fine boring cycle canned cycle? n

These values are coming form your post and as you can see high speed peck drill canned cycle is set to N for no. Setting it to this will provide the separate moves that you have already been using. So this feature would still work in your program.

So no change for fast peck.

Tapping canned cycles is set to Y. So it's using a machined canned cycle. You will need to test the cycle and let me know if it works. If you have tapped in the past successful then it would still work. If you haven't and would like to, please provide me a know working sample and definitions if needed so we can update your post.

We do provide more than 1 post processor with every purchase because customers can download post right off our website. We will make changes to your post(s), as long as you provide the information to do so. If you want us to change a post and you don't know what's wrong then well how do we know what to fix. It is the users responsibility to know their controller and the code it accepts.

Should you have to edit a post yourself, well I think so. Once you know the basic stuff by watching the V24 video I in this thread it's really not that hard to make changes that you might want. Also it's better to know how to fish then it is to just eat a fish

The bottom line is where are here to help! Not just with the BobCAD support team, but also the cnczone community. Today you were able to solve 2 issues and learn about work flow to trouble shoot others. I am sure everything you need working correctly for you post is at your finger tips, just a little testing and QA to get you where you need to be.

So test out the fast peck and tapping cycle, let me know if they work, if they don't let's fix them and get you back on track!

[ferrumdg]

Al,

I've tested it all so far...

Fastpecking works.

However Tapping is an issue - gets me the same "odd" N-thing error.

N15 G84 R G99 X85.000 Y-50.000 Z2.540 I-13.000 K0.000 F  1. S517 N1

So far I've used my Tapmatic heads and basically "normal" drilling... but as mentioned the Tapmatic things are horribly expensive. and I would much prefer to use non-reversing floating holders. but for that the tapping needs to work.

Boring gives a Syntax Error at:

N54 G86 G99 X50.000 Y-50.000 Z2.540 I-8.000 K1.200 F  3. N1

Both problems have that "N1"
From what I know - and I might be wrong - the "Nx" supposedly tells the controller to repeat that bloc Nx times... so N1 would be "one repetition".
but I'm not even sure if that is the issue because even if I manually edit the NC file to say "N3" I get the exactly same errors so it must be with the rest of the syntax? or maybe my Fagor doesn't like repeating things...


I see a bit of a pattern here - ever time the POST writes that "N1" somewhere the controller runs into some sort of an issue.



Now to the sample code.
At least according to the Fagor Programming manual for G84 and G86:


G84 - Tapping:

N0 G84 G99 G00 G91 X50 Y50 Z-98 I-22 K1.5 F350 S500 N3
N5 G98 G90 G00 X500 Y500 N1
N10 G80 G00 X0 Y0
N15 M30

G86: Boring (unfortunately the manual does not have a specific example but rather this

(G81,G82,G84,G85,G86,G89) canned cycle definition
The basic structure of the block in which one of these canned cycles is defined, is as follows:
N4 G8? G(98 or 99) (V+/-4.3) (W+/-4.3) X+/-4.3 Y+/-4.3 Z+/-4.3 I+/-4.3 K2.2 N2

What it also says is that G86 works (parameters) essentially the same as G81 to which there is an example given:

N0 G81 G98 G00 G91 X250 Y350 Z-98 I-22 F100 S500 N1
N5 G93 I250 J250
N10 A-45 N3
N15 G80 G90 X0 Y0
N20 M30

If you want the manual (I had sent this in with the custom post request originally):
https://www.dropbox.com/s/hr34o596h8...25_gp.pdf?dl=0


Let me know if you need more info.


One thing about the rest...
Yes, I don't mind modifying the post to some extent myself.
But for example programming the sequence as you did - there's no real programming reference to this and thus without that intel for example at best guess work from looking at other post files...
Also it would never have occurred to me to fix the issue this way.
I don't mind testing / sending in, etc.. .but don't expect me to perform that kind of magic on my own