[ferrumdg]

Hi

I've been using BobCAD-CAM v25 for a good bit of time now (got the 4 Axis std / 3 Axis Pro)... and use this to create code for my old Fagor 8025M controller on my 4-Axis milling machine.

Now most of the stuff works fine... but I've been running into the same problems over and over again - with no real solution provided by BobCAD.
They offered me to upgrade to v27 - but arguably I'd end up paying more for the UPGRADE than I had payed for v25 (got a good price on that one) which is bothering me, also I'm not certain that v27 will actually solve those issues as the demo doesn't come with a matching post (needed a custom post for the v25).

Reoccurring problems:

- Whenever I add a drilling operation the following operations lack the rapid Z move - the code will show "G00 " instead of "G00 Z2.54" for example... basically omitting axis & coordinate.
If I only post a single individual step - all works fine... same goes if I post the drilling separately... but as soon as it's drilling combined with other operations anything after the initial drill will slowly move Z without rapid feeding - which is often VERY slow.... So far I have "solved" this issue by manually adjusting the G00 command in the NC file..... but it is cumbersome - especially if I modify the file often enough.

- Numerous crashes
Here BobCAD support basically pointed out I should increase the time for Auto-Save intervals ... the auto save feature will do a file-save regardless of the current operation and can thus corrupt the file. Whilst increasing this to about 30 minutes has helped (I now hit "Save" much more often manually) it still didn't absolve the system from crashing ever now and again. Sometimes corrupting the file - sometimes not. It's a ll a tad unpredictable.
Mind you: the computer runs the latest windows + updates, has 12GB of Ram, 2GB Dedicated graphics memory, a reasonably fast HDD, not the latest but sufficient i3 CPU ... latest drivers, etc... so basically the PC fulfils EVERY requirement for BobCAD-CAM v25 and usually has no issues at all with anything else.

And now a weird one that has happened on numerous occasions but I can not pinpoint it down to a common denominator:
- I run a program with multiple operations (one of them being a drill)...
- The program for example does a some pockets, some profiling and then a drill...
- In the simulation all works fine.
- then I run the program on the mill and both the pocketing and profiling work as planned and as simulated. all good.
- then the drilling starts and for example is shifted by say 4mm to one side of the X Axis... Again, the pocketing, profiling, etc all worked fine.
- When I go back to bobcad-cam and simulate the thing again, all is fine - the drilling should be correct. When I choose to remove the drilling from the POST and then post it in an individual file (without the other steps, but without any changes otherwise) it will run as as it is supposed to.
Then thing is this the entire work piece of course by that time is FUBAR... (which is a tad problematic with one off custom pieces as it's a huge waste in material, time & tooling).
And sometimes this happens (with some programs) and yet it doesn't with others... it's all a bit hit / miss.



Maybe someone here has run into similar issues with v25 (or whatever) and has found a solution...

Thanks!!

[Tkamsker]

Hi I also have v25 And did let them do an linuxcnc Post for me i now found out that in can ned cycles there Are some glitches i think they Should simply fix it . I also did not möge to 27 because of cost and no Features i need ..

[ferrumdg]

Hi I also have v25 And did let them do an linuxcnc Post for me i now found out that in can ned cycles there Are some glitches i think they Should simply fix it . I also did not möge to 27 because of cost and no Features i need ..

Tkamsker

Personally I think v27 has a lot to offer - what bugs me though in this regard is that I have no reassurance that for one the mentioned problems are none existent and for another paying more for an upgrade than I paid for the original version.
I understand special deals, but what good are they if the upgrade path isn't going to keep me in the loop because of financial aspects, long term means loss of customers.

[aldepoalo]

ferrumdg,

The first issue you are having with the drill cycles is a post issue. Your post needs to be modify so that it will post the rapid move and ZR value between groups. If you wanted to email me your post I can take a look at it.

As far as crashes go, they could be caused by many things, even the auto save itself. I do not recommend auto save. What I do is every time I reach a milestone I save my file with a rev number. This way if I need to go back to earlier iterations of the file I can do so. When you auto save you loose the ability to undo past the point of the auto save..

In most cases the BobCAD system is stable, but there are "things" you can do that the software doesn't like which can result in crashes. This would be true for all CAD CAM systems. What you'll find is as you use the software more, you know what the software likes and what it doesn't like.

Now some systems will warn you about "things" you are doing that the software doesn't like and prevent crashed, like solidworks. But to be fair I've crashed solidworks many times when doing things it doesn't like. So regardless of how a crash happens, when it does and you loose work it can be very upsetting. More likely than not this is why support recommend the auto save option. Again auto save works, but I would rather control when the file is saved, and have gotten in the habit of saving at mile stones. It works for me.

If you are getting excessive crashed you should report the issue using this link.

http://bobcad.com/support/report/

Please do your best to list out the steps you take in order, with a repeatable resulted crash.

Issues like this we can track down and fix. If you can not repeat the crash with a list of steps it's very difficult for us to repeat the steps and get a crash...

Running multiple operations within a single setup or multiple setups works just fine. To me again it sounds like some issue with your post which I am guessing has some scripts in it. If I can look at the post and the file you are working on maybe I can help...

[Tkamsker]

Ferrumdg maybe it has a lot to offer but i use lathe and 3d Milling r&d stuff Light production issue is for that price (i would love to have update for Propper 4th axis and indexed 5th ) Because i am About to build 5th axis. This is simply not afford able i am About to buy madcam and rhino which gives me 2nd Option ...

[ferrumdg]

ferrumdg,

The first issue you are having with the drill cycles is a post issue. Your post needs to be modify so that it will post the rapid move and ZR value between groups. If you wanted to email me your post I can take a look at it.
...

Consider this done...
Sent you the files by mail to your gmail.

Running multiple operations within a single setup or multiple setups works just fine. To me again it sounds like some issue with your post which I am guessing has some scripts in it. If I can look at the post and the file you are working on maybe I can help...

I've attached the mentioned file to the same e-mail.
Well I ran into similar issues at different times - usually always involving drilling.
Also BobCAD CAM basically refuses to write code that runs on my Mill as soon as I combine a Center-Drill / Drill operation.
Mind you when do post those steps individually (not in succession) the program works fine... as soon as I combine it the machine gives me an error about missing sequence or something along those lines.
I had been in contact with support about this a good many times - so far without ANY solution to the problem (aside from posting the steps individually, which works, but is a huge pita).


Crashes & other issues:
See second E-Mail on it's way...
I'm not one for trying to put stuff like that out in the public...

[jrmach]

If you can attach a problem file and your PP here,you will have the power of many to solve your issues.I can pretty much guarantee you your problems are solvable.

[ferrumdg]

jrmarch,

sure - no Problem:

Post Processor (FAGOR 8025m, BobCAD-CAM 25)
https://www.dropbox.com/s/hgx88rcbme...L.MillPst?dl=0

And the file (or at least the latest one which causes the two most imminent issues: slow Z (no Rapid) and misaligned (shifted) drilling.
Mind you, that both errors only happen if all the operations are posted into one g-code file.
If you post the steps into individual output files, each step works without fail.

https://www.dropbox.com/s/wfb1z0hyoh...oor1.bbcd?dl=0

The file is just one simple part of the process (there's more to it... but it's not relevant to the problem).

[The Engine Guy]

Looked at your files and the couple of things that jump out at me are :-

1) you are mixing System and Non system tools, create all your tools at your tool library and then create a Tool Crib and populate it with the tools you want for the job, do this BEFORE you create any features, don`t fill in the tool data at the tool information page within the feature, it causes conflicts, particularly with V25 and especially drilling cycles, from my personal experience it is only a problem if you mix the tool types.

2) This line of code doesn`t look right to me :0

N4200 G43 H17 D17 Z2.54 M08

I wouldn`t normally expect to find both the H and D numbers on the same line, normally the code would have a separate line with either a G41 or G42 command and the D number as below :-

N4200 G43 H17 Z2.54 M08
N4210 G41 D17

That would normally call the Tool Height offset with the G43 line and the Tool Diameter offset (Left for G41) with the G41 line.

That`s all I have found so far, hope it is of some help

Regards
Rob
:rainfro: :rainfro: :rainfro:

[ferrumdg]

Looked at your files and the couple of things that jump out at me are :-

1) you are mixing System and Non system tools, create all your tools at your tool library and then create a Tool Crib and populate it with the tools you want for the job, do this BEFORE you create any features, don`t fill in the tool data at the tool information page within the feature, it causes conflicts, particularly with V25 and especially drilling cycles, from my personal experience it is only a problem if you mix the tool types....:

Rob,

What do you mean by "System and Non System Tools"?
I'm using a completely custom tool library that features all the tooling I have and use this to populate the Tool Crib.

Aside from that why would it be any different by adding the Tools to the Tool Crib before adding the features or from within the features??
Especially considering, that I often will figure out what specific too to use or sometimes have to change the tool after the first few runs for optimisation of the process.
And I'm really not getting "System / Non System" tools??

I will have to look into the rest (H & D) - am at home... will look into it once I'm back at the shop tomorrow.

thanks.

[aldepoalo]

Thank you for sending me your post processor and file. So the firs thing I want to look at is the post processor and the issue you have with it. To do so I am going to create a simple sample part with multiple ops.

Attachment 266572

With this part file I am going to center drill and drill the holes.
Then Pocket rough and profile finish the inside pocket
Then Profile finish the outside wall.

[aldepoalo]

All Ops posted together:

%100
N0001 ( P: BOBCAD6.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: THU. 01/29/2015)
N0004 ( TIME: 01:53PM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Center Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.1 M06
N0013G43
N0014 S4435 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 G81  X40. Y0. Z2.54 I-2.032 F324. N1
N0020 X12.361 Y38.042
N0021 X-32.361 Y23.511
N0022 Y-23.511
N0023 X12.361 Y-38.042
N0024 G00 Z5.08
N0025 Z25.4
N0026 M09
N0027 M05
(Machine Setup - 1  Drill)
(FEATURE MILL HOLE - 12.0000)
N0028 ( TOOL CHANGE )
N0029 M05
N0030 G74 Z X
N0031 T00.2 M06
N0032G43
N0033 S4107 M03
N0034 G54
N0035 G90
N0036 X40. Y0.
N0037 M08
N0038 G00 Z5.08
N0039 G81  X40. Y0. Z2.54 I-13.605 F300. N1
N0040 X12.361 Y38.042
N0041 X-32.361 Y23.511
N0042 Y-23.511
N0043 X12.361 Y-38.042
N0044 G00 Z5.08
N0045 Z25.4
N0046 M09
N0047 M05
(Machine Setup - 1  Pocket)
(FEATURE 2 AXIS)
N0048 ( TOOL CHANGE )
N0049 M05
N0050 G74 Z X
N0051 T00.3 M06
N0052G43
N0053 S9857 M03
N0054 G54
N0055 G90
N0056 X2.119 Y0.
N0057 M08
N0058 G00 Z5.08
N0059 Z2.54
N0060 G01 Z0. F2879.
N0061 Z-12.7
N0062 G17 G03 X-2.119 Y0. R2.119 F5759.
N0063 G03 X2.119 Y0. R2.119
N0064 G01 X4.619
N0065 G03 X-4.619 Y0. R4.619
N0066 G03 X4.619 Y0. R4.619
N0067 G01 X7.119
N0068 G03 X-7.119 Y0. R7.119
N0069 G03 X7.119 Y0. R7.119
N0070 G01 X9.619
N0071 G03 X-9.619 Y0. R9.619
N0072 G03 X9.619 Y0. R9.619
N0073 G01 X12.119
N0074 G03 X-12.119 Y0. R12.119
N0075 G03 X12.119 Y0. R12.119
N0076 G01 X14.619
N0077 G03 X-14.619 Y0. R14.619
N0078 G03 X14.619 Y0. R14.619
N0079 G01 X17.119
N0080 G03 X-17.119 Y0. R17.119
N0081 G03 X17.119 Y0. R17.119
N0082 G01 X19.619
N0083 G03 X-19.619 Y0. R19.619
N0084 G03 X19.619 Y0. R19.619
N0085 G01 X22.119
N0086 G03 X-22.119 Y0. R22.119
N0087 G03 X22.119 Y0. R22.119
N0088 G01 X24.619
N0089 G03 X-24.619 Y0. R24.619
N0090 G03 X24.619 Y0. R24.619
N0091 G01 X27.119
N0092 G03 X-27.119 Y0. R27.119
N0093 G03 X27.119 Y0. R27.119
N0094 G00 Z5.08
N0095 Z25.4
N0096 M09
N0097 M05
(Machine Setup - 1  Profile Finish)
(FEATURE 2 AXIS)
N0098 ( TOOL CHANGE )
N0099 M05
N0100 G74 Z X
N0101 T00.4 M06
N0102G43
N0103 S9857 M03
N0104 G54
N0105 G90
N0106 X21.15 Y0.
N0107 M08
N0108 G00 Z5.08
N0109 Z2.54
N0110 G01 Z-12.7 F1440.
N0111 Y-6.35 F2879.
N0112 G17 G03 X27.5 Y0. R6.35
N0113 G03 X-27.5 Y0. R27.5
N0114 G03 X27.5 Y0. R27.5
N0115 G03 X21.15 Y6.35 R6.35
N0116 G01 Y0.
N0117 G00 Z5.08
N0118 Z25.4
(Machine Setup - 1  Profile Finish)
(FEATURE 2 AXIS)
N0119 S9857
N0120 G54
N0121 G90
N0122 X-58.85 Y40.
N0123 Z5.08
N0124 Z2.54
N0125 G01 Z-5. F1440.
N0126 Y33.65 F2879.
N0127 G03 X-52.5 Y40. R6.35
N0128 G02 X-40. Y52.5 R12.5
N0129 G01 X40.
N0130 G02 X52.5 Y40. R12.5
N0131 G01 Y-40.
N0132 G02 X40. Y-52.5 R12.5
N0133 G01 X-40.
N0134 G02 X-52.5 Y-40. R12.5
N0135 G01 Y40.
N0136 G03 X-58.85 Y46.35 R6.35
N0137 G01 Y40.
N0138 G00 Z5.08
N0139 Z25.4
N0140 M09
N0141 M05
N0142 G74 Z X
N0143 M30

Just Drill Cycles posted together:

%100
N0001 ( P: BOBCAD6.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: THU. 01/29/2015)
N0004 ( TIME: 01:54PM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Center Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.1 M06
N0013G43
N0014 S4435 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 G81  X40. Y0. Z2.54 I-2.032 F324. N1
N0020 X12.361 Y38.042
N0021 X-32.361 Y23.511
N0022 Y-23.511
N0023 X12.361 Y-38.042
N0024 G00 Z5.08
N0025 Z25.4
N0026 M09
N0027 M05
(Machine Setup - 1  Drill)
(FEATURE MILL HOLE - 12.0000)
N0028 ( TOOL CHANGE )
N0029 M05
N0030 G74 Z X
N0031 T00.2 M06
N0032G43
N0033 S4107 M03
N0034 G54
N0035 G90
N0036 X40. Y0.
N0037 M08
N0038 G00 Z5.08
N0039 G81  X40. Y0. Z2.54 I-13.605 F300. N1
N0040 X12.361 Y38.042
N0041 X-32.361 Y23.511
N0042 Y-23.511
N0043 X12.361 Y-38.042
N0044 G00 Z5.08
N0045 Z25.4
N0046 M09
N0047 M05
N0048 G74 Z X
N0049 M30

Drill cycles posted separately:

Center Drill:

%100
N0001 ( P: BOBCAD6.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: THU. 01/29/2015)
N0004 ( TIME: 01:55PM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Center Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.1 M06
N0013G43
N0014 S4435 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 G81  X40. Y0. Z2.54 I-2.032 F324. N1
N0020 X12.361 Y38.042
N0021 X-32.361 Y23.511
N0022 Y-23.511
N0023 X12.361 Y-38.042
N0024 G00 Z5.08
N0025 Z25.4
N0026 M09
N0027 M05
N0028 G74 Z X
N0029 M30

Drill:

%100
N0001 ( P: BOBCAD6.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: THU. 01/29/2015)
N0004 ( TIME: 01:56PM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.2 M06
N0013G43
N0014 S4107 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 G81  X40. Y0. Z2.54 I-13.605 F300. N1
N0020 X12.361 Y38.042
N0021 X-32.361 Y23.511
N0022 Y-23.511
N0023 X12.361 Y-38.042
N0024 G00 Z5.08
N0025 Z25.4
N0026 M09
N0027 M05
N0028 G74 Z X
N0029 M30

[The Engine Guy]

In some of your features you have unchecked the box for "System Tools" and then the information boxes will have changed from being mostly "greyed out" to White and you are able to fill in the boxes and in effect create a tool, in the past conflicts have arisen when a user has used a mixture of tools created in the feature and tools created in the Library which usually populate the tool info area automatically.

No one seems to know why it happened although I haven`t seen any such issues with V26 or V27, although fair to say I now NEVER try to create tools in the feature tool info area, I ALWAYS create them in the Tool Library and then load them into the Tool Crib that I have created for the particular job.

I name/number all the Cribs I create and keep a log of what tools are in each Crib, often I can just load an existing Crib for a new job and maybe add or drop the odd tool and I`m usually good to go, I find it works for me and save loads of time and effort

regards
Rob
:rainfro: :rainfro: :rainfro:

[aldepoalo]

After getting more information from ferrumdg, I understand the issue with posting happens when using a pecking cycle and having more than 1 op. So let's look at the code and see what is going on.

Here is a peck cycle by itself:

%100
N0001 ( P: CNC ZONE GUY.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 09:13AM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.2 M06
N0013G43
N0014 S4107 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 Z2.54
N0020 G01 Z-3.46 F300.
N0021 G00 Z2.54
N0022 Z-0.92
N0023 G01 Z-9.46
N0024 G00 Z2.54
N0025 Z-6.92
N0026 G01 Z-13.605
N0027 G00 Z2.54
N0028 Z5.08
N0029 X12.361 Y38.042
N0030 Z2.54
N0031 G01 Z-3.46 F300.
N0032 G00 Z2.54
N0033 Z-0.92
N0034 G01 Z-9.46
N0035 G00 Z2.54
N0036 Z-6.92
N0037 G01 Z-13.605
N0038 G00 Z2.54
N0039 Z5.08
N0040 X-32.361 Y23.511
N0041 Z2.54
N0042 G01 Z-3.46 F300.
N0043 G00 Z2.54
N0044 Z-0.92
N0045 G01 Z-9.46
N0046 G00 Z2.54
N0047 Z-6.92
N0048 G01 Z-13.605
N0049 G00 Z2.54
N0050 Z5.08
N0051 Y-23.511
N0052 Z2.54
N0053 G01 Z-3.46 F300.
N0054 G00 Z2.54
N0055 Z-0.92
N0056 G01 Z-9.46
N0057 G00 Z2.54
N0058 Z-6.92
N0059 G01 Z-13.605
N0060 G00 Z2.54
N0061 Z5.08
N0062 X12.361 Y-38.042
N0063 Z2.54
N0064 G01 Z-3.46 F300.
N0065 G00 Z2.54
N0066 Z-0.92
N0067 G01 Z-9.46
N0068 G00 Z2.54
N0069 Z-6.92
N0070 G01 Z-13.605
N0071 G00 Z2.54
N0072 Z5.08
N0073 Z25.4
N0074 M09
N0075 M05
N0076 G74 Z X
N0077 M30

Here is a peck cycle with a pocketing op:

%100
N0001 ( P: CNC ZONE GUY.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 09:17AM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.2 M06
N0013G43
N0014 S4107 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 Z2.54
N0020 G01 Z-3.46 F300.
N0021 G00 Z2.54
N0022 Z-0.92
N0023 G01 Z-9.46
N0024 G00 Z2.54
N0025 Z-6.92
N0026 G01 Z-13.605
N0027 G00 Z2.54
N0028 Z5.08
N0029 X12.361 Y38.042
N0030 Z2.54
N0031 G01 Z-3.46 F300.
N0032 G00 Z2.54
N0033 Z-0.92
N0034 G01 Z-9.46
N0035 G00 Z2.54
N0036 Z-6.92
N0037 G01 Z-13.605
N0038 G00 Z2.54
N0039 Z5.08
N0040 X-32.361 Y23.511
N0041 Z2.54
N0042 G01 Z-3.46 F300.
N0043 G00 Z2.54
N0044 Z-0.92
N0045 G01 Z-9.46
N0046 G00 Z2.54
N0047 Z-6.92
N0048 G01 Z-13.605
N0049 G00 Z2.54
N0050 Z5.08
N0051 Y-23.511
N0052 Z2.54
N0053 G01 Z-3.46 F300.
N0054 G00 Z2.54
N0055 Z-0.92
N0056 G01 Z-9.46
N0057 G00 Z2.54
N0058 Z-6.92
N0059 G01 Z-13.605
N0060 G00 Z2.54
N0061 Z5.08
N0062 X12.361 Y-38.042
N0063 Z2.54
N0064 G01 Z-3.46 F300.
N0065 G00 Z2.54
N0066 Z-0.92
N0067 G01 Z-9.46
N0068 G00 Z2.54
N0069 Z-6.92
N0070 G01 Z-13.605
N0071 G00 Z2.54
N0072 Z5.08
N0073 Z25.4
N0074 M09
N0075 M05
(Machine Setup - 1  Pocket)
(FEATURE 2 AXIS)
N0076 ( TOOL CHANGE )
N0077 M05
N0078 G74 Z X
N0079 T00.3 M06
N0080G43
N0081 S9857 M03
N0082 G54
N0083 G90
N0084 X2.119 Y0.
N0085 M08
N0086 G00 Z5.08
N0087 Z2.54
N0088 G01 Z0. F2879.
N0089 Z-12.7
N0090 G17 G03 X-2.119 Y0. R2.119 F5759.
N0091 G03 X2.119 Y0. R2.119
N0092 G01 X4.619
N0093 G03 X-4.619 Y0. R4.619
N0094 G03 X4.619 Y0. R4.619
N0095 G01 X7.119
N0096 G03 X-7.119 Y0. R7.119
N0097 G03 X7.119 Y0. R7.119
N0098 G01 X9.619
N0099 G03 X-9.619 Y0. R9.619
N0100 G03 X9.619 Y0. R9.619
N0101 G01 X12.119
N0102 G03 X-12.119 Y0. R12.119
N0103 G03 X12.119 Y0. R12.119
N0104 G01 X14.619
N0105 G03 X-14.619 Y0. R14.619
N0106 G03 X14.619 Y0. R14.619
N0107 G01 X17.119
N0108 G03 X-17.119 Y0. R17.119
N0109 G03 X17.119 Y0. R17.119
N0110 G01 X19.619
N0111 G03 X-19.619 Y0. R19.619
N0112 G03 X19.619 Y0. R19.619
N0113 G01 X22.119
N0114 G03 X-22.119 Y0. R22.119
N0115 G03 X22.119 Y0. R22.119
N0116 G01 X24.619
N0117 G03 X-24.619 Y0. R24.619
N0118 G03 X24.619 Y0. R24.619
N0119 G01 X27.119
N0120 G03 X-27.119 Y0. R27.119
N0121 G03 X27.119 Y0. R27.119
N0122 G00 Z5.08
N0123 Z25.4
N0124 M09
N0125 M05
N0126 G74 Z X
N0127 M30

Here is the complete sample like I posted before, the only change is using a pecking cycle:

%100
N0001 ( P: CNC ZONE GUY.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 09:18AM)
N0005 G90 G80 G71 G40 G17
N0006 (Machine Setup - 1  Center Drill)
N0007 (FEATURE MILL HOLE - 12.0000)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.1 M06
N0013G43
N0014 S4435 M03
N0015 G54
N0016 G00 G90 X40. Y0. Z25.4
N0017 M08
N0018 Z5.08
N0019 G81  X40. Y0. Z2.54 I-2.032 F324. N1
N0020 X12.361 Y38.042
N0021 X-32.361 Y23.511
N0022 Y-23.511
N0023 X12.361 Y-38.042
N0024 G00 Z5.08
N0025 Z25.4
N0026 M09
N0027 M05
(Machine Setup - 1  Drill)
(FEATURE MILL HOLE - 12.0000)
N0028 ( TOOL CHANGE )
N0029 M05
N0030 G74 Z X
N0031 T00.2 M06
N0032G43
N0033 S4107 M03
N0034 G54
N0035 G90
N0036 X40. Y0.
N0037 M08
N0038 G00 Z5.08
N0039 Z2.54
N0040 G01 Z-3.46 F300.
N0041 G00 Z2.54
N0042 Z-0.92
N0043 G01 Z-9.46
N0044 G00 Z2.54
N0045 Z-6.92
N0046 G01 Z-13.605
N0047 G00 Z2.54
N0048 Z5.08
N0049 X12.361 Y38.042
N0050 Z2.54
N0051 G01 Z-3.46 F300.
N0052 G00 Z2.54
N0053 Z-0.92
N0054 G01 Z-9.46
N0055 G00 Z2.54
N0056 Z-6.92
N0057 G01 Z-13.605
N0058 G00 Z2.54
N0059 Z5.08
N0060 X-32.361 Y23.511
N0061 Z2.54
N0062 G01 Z-3.46 F300.
N0063 G00 Z2.54
N0064 Z-0.92
N0065 G01 Z-9.46
N0066 G00 Z2.54
N0067 Z-6.92
N0068 G01 Z-13.605
N0069 G00 Z2.54
N0070 Z5.08
N0071 Y-23.511
N0072 Z2.54
N0073 G01 Z-3.46 F300.
N0074 G00 Z2.54
N0075 Z-0.92
N0076 G01 Z-9.46
N0077 G00 Z2.54
N0078 Z-6.92
N0079 G01 Z-13.605
N0080 G00 Z2.54
N0081 Z5.08
N0082 X12.361 Y-38.042
N0083 Z2.54
N0084 G01 Z-3.46 F300.
N0085 G00 Z2.54
N0086 Z-0.92
N0087 G01 Z-9.46
N0088 G00 Z2.54
N0089 Z-6.92
N0090 G01 Z-13.605
N0091 G00 Z2.54
N0092 Z5.08
N0093 Z25.4
N0094 M09
N0095 M05
(Machine Setup - 1  Pocket)
(FEATURE 2 AXIS)
N0096 ( TOOL CHANGE )
N0097 M05
N0098 G74 Z X
N0099 T00.3 M06
N0100G43
N0101 S9857 M03
N0102 G54
N0103 G90
N0104 X2.119 Y0.
N0105 M08
N0106 G00 Z5.08
N0107 Z2.54
N0108 G01 Z0. F2879.
N0109 Z-12.7
N0110 G17 G03 X-2.119 Y0. R2.119 F5759.
N0111 G03 X2.119 Y0. R2.119
N0112 G01 X4.619
N0113 G03 X-4.619 Y0. R4.619
N0114 G03 X4.619 Y0. R4.619
N0115 G01 X7.119
N0116 G03 X-7.119 Y0. R7.119
N0117 G03 X7.119 Y0. R7.119
N0118 G01 X9.619
N0119 G03 X-9.619 Y0. R9.619
N0120 G03 X9.619 Y0. R9.619
N0121 G01 X12.119
N0122 G03 X-12.119 Y0. R12.119
N0123 G03 X12.119 Y0. R12.119
N0124 G01 X14.619
N0125 G03 X-14.619 Y0. R14.619
N0126 G03 X14.619 Y0. R14.619
N0127 G01 X17.119
N0128 G03 X-17.119 Y0. R17.119
N0129 G03 X17.119 Y0. R17.119
N0130 G01 X19.619
N0131 G03 X-19.619 Y0. R19.619
N0132 G03 X19.619 Y0. R19.619
N0133 G01 X22.119
N0134 G03 X-22.119 Y0. R22.119
N0135 G03 X22.119 Y0. R22.119
N0136 G01 X24.619
N0137 G03 X-24.619 Y0. R24.619
N0138 G03 X24.619 Y0. R24.619
N0139 G01 X27.119
N0140 G03 X-27.119 Y0. R27.119
N0141 G03 X27.119 Y0. R27.119
N0142 G00 Z5.08
N0143 Z25.4
N0144 M09
N0145 M05
(Machine Setup - 1  Profile Finish)
(FEATURE 2 AXIS)
N0146 ( TOOL CHANGE )
N0147 M05
N0148 G74 Z X
N0149 T00.4 M06
N0150G43
N0151 S9857 M03
N0152 G54
N0153 G90
N0154 X21.15 Y0.
N0155 M08
N0156 G00 Z5.08
N0157 Z2.54
N0158 G01 Z-12.7 F1440.
N0159 Y-6.35 F2879.
N0160 G17 G03 X27.5 Y0. R6.35
N0161 G03 X-27.5 Y0. R27.5
N0162 G03 X27.5 Y0. R27.5
N0163 G03 X21.15 Y6.35 R6.35
N0164 G01 Y0.
N0165 G00 Z5.08
N0166 Z25.4
(Machine Setup - 1  Profile Finish)
(FEATURE 2 AXIS)
N0167 S9857
N0168 G54
N0169 G90
N0170 X-58.85 Y40.
N0171 Z5.08
N0172 Z2.54
N0173 G01 Z-5. F1440.
N0174 Y33.65 F2879.
N0175 G03 X-52.5 Y40. R6.35
N0176 G02 X-40. Y52.5 R12.5
N0177 G01 X40.
N0178 G02 X52.5 Y40. R12.5
N0179 G01 Y-40.
N0180 G02 X40. Y-52.5 R12.5
N0181 G01 X-40.
N0182 G02 X-52.5 Y-40. R12.5
N0183 G01 Y40.
N0184 G03 X-58.85 Y46.35 R6.35
N0185 G01 Y40.
N0186 G00 Z5.08
N0187 Z25.4
N0188 M09
N0189 M05
N0190 G74 Z X
N0191 M30

[aldepoalo]

Ok, so now that we have some code up, from what I can tell I do not see an issue with the code when posted as a single op or posted with other ops. In other words the code looks the same to me when by itself or posted in a group of ops...

Now you do notice that the peck cycle using separate moves, not a canned cycle. The reason why is fagor uses an non tradition peck cycle that requires some scripting to post the code in the correct format. Recently ( in the last few month ) I know we ( bobcad) worked on a fagor post to support the canned cycle for pecking. As far as I know the post was made for V25, but I'll have to check.

So the question is, what is the problem you are having with the code? You are saying it's not going to clearance between operations? Can you provide a little more details about the problem so we can get it sorted out?

[ferrumdg]

In some of your features you have unchecked the box for "System Tools" and then the information boxes will have changed from being mostly "greyed out" to White and you are able to fill in the boxes and in effect create a tool, in the past conflicts have arisen when a user has used a mixture of tools created in the feature and tools created in the Library which usually populate the tool info area automatically.

No one seems to know why it happened although I haven`t seen any such issues with V26 or V27, although fair to say I now NEVER try to create tools in the feature tool info area, I ALWAYS create them in the Tool Library and then load them into the Tool Crib that I have created for the particular job.

I name/number all the Cribs I create and keep a log of what tools are in each Crib, often I can just load an existing Crib for a new job and maybe add or drop the odd tool and I`m usually good to go, I find it works for me and save loads of time and effort

regards
Rob
:rainfro: :rainfro: :rainfro:

Rob

Thank you - but it makes no sense to me (System Tools)...

I do NOT create tools on the go... all the tools I use I do indeed select from the "Tool Crib"!
Î've noticed the "System Tool" checkbox and it has honestly not made much sense to me...
Whenever I add a tool from the Tool Crib - it will by default UNCHEK "System Tool".
I do not manually modify or create the tools after adding them - not at all... all tools defined originally in the Tool Library (although I use a custom library as the default tools are of no use for me). Then added from the Library to the Tool Crib.

The only thing I do indeed deactivate manually is the "Automatic Tool Numbering" - as that wreaks havoc. My machine requires the tool numbers as defined in the Tool Library by myself. Can't do any of that Auto Numbering thing.

So no - I don't mix manually created tools and Library tools... actually I never use manually edited tools anyhow.

[ferrumdg]

Ok, so now that we have some code up, from what I can tell I do not see an issue with the code when posted as a single op or posted with other ops. In other words the code looks the same to me when by itself or posted in a group of ops...

Now you do notice that the peck cycle using separate moves, not a canned cycle. The reason why is fagor uses an non tradition peck cycle that requires some scripting to post the code in the correct format. Recently ( in the last few month ) I know we ( bobcad) worked on a fagor post to support the canned cycle for pecking. As far as I know the post was made for V25, but I'll have to check.

So the question is, what is the problem you are having with the code? You are saying it's not going to clearance between operations? Can you provide a little more details about the problem so we can get it sorted out?

As mentioned before:
(from my last e-Mail):

The issue is two things:
Both issues have one common aspect: DRILLING.
Neither issue happens unless a drilling (pecking or fast peck) is implemented.

1) This one is easy to replicate as it happens EVERY time
After a drilling operation all following features lack a RAPID Z move and basically from the Tool change on will move the Z Axis at regular feed speeds down to the the work piece (which of course takes forever).


2) this one is tricky as it is an on/off thing that happens occasionally and I have not been able to pin-point it to something specific.
Shifted holes.
Again this is inconsistent but far more worrisome due to its unpredictable nature.
It happens with the script I had sent you.
Run as an entire program in one file: the drilled holes are offset on the X Axis from what they're supposed to be (looks good both on the drawing, tool paths and the simulation though).
When I post the features individually it works without fail though.
Has happened a few times to this day and I can't nail it to anything specific. Has actually ruined a few pieces....

3) If run a center drill followed by a drill - the step after that will be "broken".
Consistently happening.
Basically the controller looks for an odd Sequence number and tries to "jump".
But NOWHERE in the code is either a sub-routine or even a Call of such a sequence...


From the file I had posted originally:

N421 M09
N422 M05
N423 ( TOOL CHANGE )
N424 M05
N425 G74 Z X
N426 T00.17 M06
N427 G43
N428 S6000 M03
N429 G90
N430 X10.091 Y-6.680
N431 M08
N432 G01 Z1.880 F120.
N433 G00 Z2.540
N434 Z4.420
N435 G01 Z0.230
N436 G00 Z2.540
N437 Z2.770
N438 G01 Z-1.420
N439 G00 Z2.540
N440 Z1.120
N441 G01 Z-3.070
N442 G00 Z2.540
N443 Z-0.530
N444 G01 Z-4.720
N445 G00 Z2.540
N446 Z-2.180
N447 G01 Z-6.370
N448 G00 Z2.540
N449 Z-3.830
N450 G01 Z-8.020
N451 G00 Z2.540
N452 Z-5.480
N453 G01 Z-8.261
N454 G00 Z2.540
N455 X6.949 Y-50.604
N456 G01 Z1.880
N457 G00 Z2.540
N458 Z4.420
N459 G01 Z0.230
N460 G00 Z2.540
N461 Z2.770
N462 G01 Z-1.420
N463 G00 Z2.540
N464 Z1.120
N465 G01 Z-3.070
N466 G00 Z2.540
N467 Z-0.530
N468 G01 Z-4.720
N469 G00 Z2.540
N470 Z-2.180
N471 G01 Z-6.370
N472 G00 Z2.540
N473 Z-3.830
N474 G01 Z-8.020
N475 G00 Z2.540
N476 Z-5.480
N477 G01 Z-8.261
N478 G00 Z2.540
N479 X4.182 Y-95.009
N480 G01 Z1.880
N481 G00 Z2.540
N482 Z4.420
N483 G01 Z0.230
N484 G00 Z2.540
N485 Z2.770
N486 G01 Z-1.420
N487 G00 Z2.540
N488 Z1.120
N489 G01 Z-3.070
N490 G00 Z2.540
N491 Z-0.530
N492 G01 Z-4.720
N493 G00 Z2.540
N494 Z-2.180
N495 G01 Z-6.370
N496 G00 Z2.540
N497 Z-3.830
N498 G01 Z-8.020
N499 G00 Z2.540
N500 Z-5.480
N501 G01 Z-8.261
N502 G00 Z2.540
N503 M09
N504 M05
N505 ( TOOL CHANGE )
N506 M05
N507 G74 Z X
N508 T00.12 M06
N509 G43
N510 S6000 M03
N511 G90
N512 X3.080 Y-112.671
N513 M08
N514 G00
N515 G01 Z-7.000 F 95.

As is apparent on the N433 Line - it does indeed do a RAPID move (G00 Z2.54) to Z 2.54
In the BobCad file (marcel_outdoor1...) I had attached this is the SECOND FEATURE (drilling with Tool 17)...

Now when it changes tool again for the Next Feature (from N505 onwards) you will see on line N514 a command that says: "G00" and nothing more.
So it wants to do the RAPID move that it should (again down to 2.54) but for some weird reason completely ommits the VALUE (Coord.).

And it does so EVERY time I implement a DRILLING routing for EVERY following feature (but not for the drilling itself).
Unless I post the features as individual unique files - than it works.

[aldepoalo]

Ok so let's take one issue at a time.

1) This one is easy to replicate as it happens EVERY time
After a drilling operation all following features lack a RAPID Z move and basically from the Tool change on will move the Z Axis at regular feed speeds down to the the work piece (which of course takes forever).


Here is the code for the end of the drilling cycle then a tool call for the pocket cycle.

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 G00
N0102 G01 Z-7. F 95.  <<<<<<<<<<<<<<<<<

Here is the same code with the post processor debug on:

N0088 G00 Z2.54
************* 40 - Operations//Start of operation **********
************* 3 - Tool Change//Move to next cut change tool **********
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
************* 40 - Operations//Start of operation **********
************* 27 - Rapid moves//First rapid move Z **********
N0101 G00
************* 51 - Feed moves//Feed move Z **********
N0102 G01 Z-7. F 95.

So the feed problem that is concurring, after a tool change is happening in your post block 3, So let's look at the code from the post.

3. Tool change
	n,coolant_off
	n,spindle_off
	system_comment
	feature_name_comment
	n,"( TOOL CHANGE )"
	n,spindle_off
	n,coolant_off
	n,"G74 Z X"
	n_forced,"T00.",list_tool_number,"M06"
	n,output_rotary_angle
  n,output_second_rotary_angle
	n,length_offset
	n,s,spindle_on
	n,work_coord
	n,rapid_move,absolute_coord
	n,force_x,xr,force_y,yr,p_rot,s_rot,
	n,coolant_on
	output_rotary_angle

In this block of code you can see after the work cord and the force XY move you do not see anything for Z. So what is happening is the software still thinks it's at it's last Z move which is N0088 G00 Z2.54 and because there is nothing in the code to tell the tool to come down to Z after the tool change. The fist Z move is a feed move. So the tool is feeding from the Z tool change location.

The good thing about this issue is it's easy to fix and also will not create scrap, it just extends the run time.

You should be thinking why isn't a Z move posted on N0101 G00 This is because your code is model and the last Z move was at G00 Z2.54 so it doesn't post this location again because there was no change.

What we need to do to fix this is force a Z move in the tool change block to bring the tool back down to clearance as a rapid move.

3. Tool change
	n,coolant_off
	n,spindle_off
	system_comment
	feature_name_comment
	n,"( TOOL CHANGE )"
	n,spindle_off
	n,coolant_off
	n,"G74 Z X"
	n_forced,"T00.",list_tool_number,"M06"
	n,output_rotary_angle
  n,output_second_rotary_angle
	n,length_offset
	n,s,spindle_on
	n,work_coord
	n,rapid_move,absolute_coord
	n,force_x,xr,force_y,yr,p_rot,s_rot,
	n,coolant_on
	n,force_z,zr  <<<<<<<<<<<<<<<<<<<<<<<
	output_rotary_angle

Adding the force_z,zr will force a Z move and bring the tool down to the clearance plane after the tool had moved to it's next XY location.


Now that I've made this change to the post this is what the code looks like:

Code with debug on:

N0088 G00 Z2.54
************* 40 - Operations//Start of operation **********
************* 3 - Tool Change//Move to next cut change tool **********
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
************* 40 - Operations//Start of operation **********
************* 27 - Rapid moves//First rapid move Z **********
N0102 G00
************* 51 - Feed moves//Feed move Z **********
N0103 G01 Z-7. F 95.

Code with debug off:

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
N0103 G01 Z-7. F 95.

So that was a simple fix....


The other thing I noticed is on your posting block #2 that you work cord reference moves looks like this.

n,rapid_move,absolute_coord,force_x,xr,force_y,yr, zr,p_rot,s_rot


This will create a ramp move to your start location. I personally do not like this even if it's faster... I would prefer to have the XY move at tool change Z and once in location have the tool come down.

So I would change the post block to :

n,rapid_move,absolute_coord,force_x,xr,force_y,yr, p_rot,s_rot
n,rapid_move, force_z,zr

[aldepoalo]

So now let's look at shifted holes.

2) this one is tricky as it is an on/off thing that happens occasionally and I have not been able to pin-point it to something specific.
Shifted holes.
Again this is inconsistent but far more worrisome due to its unpredictable nature.
It happens with the script I had sent you.
Run as an entire program in one file: the drilled holes are offset on the X Axis from what they're supposed to be (looks good both on the drawing, tool paths and the simulation though).
When I post the features individually it works without fail though.
Has happened a few times to this day and I can't nail it to anything specific. Has actually ruined a few pieces....

Here are the hole locations based on your drawing you send me relative to part origin:

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

Ok so now let's look at the posted code from the script you sent me. (In this case when we say script we are talking about the g -code )

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


What you find is the hole locations match the drawing locations. So the problem you are having is not the drawing the code BobCAD is creating. BobCAD will post the locations of holes as defined by your drawing.. So what's going on here, why is it that some times you holes are shifted slightly?

I am not sure but I have 2 ideas.

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.

[aldepoalo]

Let's now take a look at the 3rd question:


3) If run a center drill followed by a drill - the step after that will be "broken".
Consistently happening.
Basically the controller looks for an odd Sequence number and tries to "jump".
But NOWHERE in the code is either a sub-routine or even a Call of such a sequence...


Posted code with center drill and drill op:

%100
N0001 ( P: MARCEL_OUTDOOR1.NC)
N0002 ( POST:  FAGOR 8025M METRIC)
N0003 ( DATE: FRI. 01/30/2015)
N0004 ( TIME: 10:39AM)
N0005 G90 G80 G71 G40 G17
N0006 (JOB 2  CENTER HOLE  RANDOM POINT PATTERN)
N0007 (FEATURE CENTER DRILL)
N0008 ( TOOL CHANGE )
N0009 M05
N0010 G44
N0011 G74 Z X
N0012 T00.1 M06
N0013G43
N0014 S6000 M03
N0015 G54
N0016 G00 G90 X-10.091 Y6.68 Z2.54
N0017 M08
N0018 G81 G99 X-10.091 Y6.68 Z2.54 I-0.635 F178. N1
N0019 X-6.949 Y50.604
N0020 X-4.182 Y95.009
N0021 M09
N0022 M05
(JOB 3  HOLE  RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)
N0023 ( TOOL CHANGE )
N0024 M05
N0025 G74 Z X
N0026 T00.17 M06
N0027G43
N0028 S6000 M03
N0029 G54
N0030 G00 G90
N0031 X-10.091 Y6.68
N0032 M08
N0033 Z2.54
N0034 G01 Z1.88 F120.
N0035 G00 Z2.54
N0036 Z4.42
N0037 G01 Z0.23
N0038 G00 Z2.54
N0039 Z2.77
N0040 G01 Z-1.42
N0041 G00 Z2.54
N0042 Z1.12
N0043 G01 Z-3.07
N0044 G00 Z2.54
N0045 Z-0.53
N0046 G01 Z-4.72
N0047 G00 Z2.54
N0048 Z-2.18
N0049 G01 Z-6.37
N0050 G00 Z2.54
N0051 Z-3.83
N0052 G01 Z-8.02
N0053 G00 Z2.54
N0054 Z-5.48
N0055 G01 Z-8.261
N0056 G00 Z2.54
N0057 X-6.949 Y50.604
N0058 G01 Z1.88
N0059 G00 Z2.54
N0060 Z4.42
N0061 G01 Z0.23
N0062 G00 Z2.54
N0063 Z2.77
N0064 G01 Z-1.42
N0065 G00 Z2.54
N0066 Z1.12
N0067 G01 Z-3.07
N0068 G00 Z2.54
N0069 Z-0.53
N0070 G01 Z-4.72
N0071 G00 Z2.54
N0072 Z-2.18
N0073 G01 Z-6.37
N0074 G00 Z2.54
N0075 Z-3.83
N0076 G01 Z-8.02
N0077 G00 Z2.54
N0078 Z-5.48
N0079 G01 Z-8.261
N0080 G00 Z2.54
N0081 X-4.182 Y95.009
N0082 G01 Z1.88
N0083 G00 Z2.54
N0084 Z4.42
N0085 G01 Z0.23
N0086 G00 Z2.54
N0087 Z2.77
N0088 G01 Z-1.42
N0089 G00 Z2.54
N0090 Z1.12
N0091 G01 Z-3.07
N0092 G00 Z2.54
N0093 Z-0.53
N0094 G01 Z-4.72
N0095 G00 Z2.54
N0096 Z-2.18
N0097 G01 Z-6.37
N0098 G00 Z2.54
N0099 Z-3.83
N0100 G01 Z-8.02
N0101 G00 Z2.54
N0102 Z-5.48
N0103 G01 Z-8.261
N0104 G00 Z2.54
N0105 M09
N0106 M05
N0107 G74 Z X
N0108 M30

The problem I think you are asking about is not the center drill but the G81 canned cycle. Let' take a look at the posting blocks for this.

N0016 G00 G90 X-10.091 Y6.68 Z2.54
N0017 M08
************* 81 - Canned cycles//Standard drill **********
************* 22 - Misc//Rigid tapping start **********
N0018 G81 G99 X-10.091 Y6.68 Z2.54 I-0.635 F178. N1
************* 91 - Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS. **********
N0019 X-6.949 Y50.604
************* 91 - Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS. **********
N0020 X-4.182 Y95.009
************* 80 - Canned cycles//Canned cycle cancel **********
************* 40 - Operations//Start of operation **********
************* 3 - Tool Change//Move to next cut change tool **********
N0021 M09
N0022 M05

81. Standard drill canned cycle.
	rigid_tapping_start
	n,g_canned_cycle,g98_g99,x_f,y_f,reference_plane,drill_depth,canned_feed_rate,"N1"

My gut it telling me that canned cycles for this post are not setup correctly and the "N1" has something to do with your "broken " problem. In order to really know what is going on with the canned cycle I would need to see a working program and definition of variables / format.

What I think your g-code should look like is more like this:

%000100,MX,
N1 G90 G80 G70 G40 G17
;JOB 2  CENTER HOLE  RANDOM POINT PATTERN
;FEATURE CENTER DRILL
N2 T1 M06
N3 S10000 M03
N4 G53
N5 G54
N6 G00 X-10.0912 Y6.6797
N7 G43 Z2.54 D1
N8 M08
N9 G81 G98 X-10.0912 Y6.6797 Z2.54 I-0.635 F177.8
N10 X-6.9491 Y50.6042
N11 X-4.182 Y95.009
N12 G80
N13 M09
N14 M05
;JOB 3  HOLE  RANDOM POINT PATTERN
;FEATURE DRILL HOLE
N15 T17 M06
N16 S6000 M03
N17 G53
N18 G54
N19 G00 X-10.091 Y6.68
N20 G43 Z2.54 D17
N21 M08
N22 G83 G98 X-10.091 Y6.68 Z2.54 I-1.377 J6 F120.
N23 X-6.949 Y50.604
N24 X-4.182 Y95.009
N25 G80
N26 M09
N27 M05
N28 T1 M06
N29 M30

In this case we are using canned cycles and I think the peck cycle works correctly because we have scripted a posting block to handle it correctly.

Posting block for G81

81. Standard drill canned cycle.
	rigid_tapping_start
	n,g_canned_cycle,g98_g99,x_f,y_f,reference_plane,drill_depth,canned_feed_rate

Posting Block for G83

83. Peck drill canned cycle.
	rigid_tapping_start
	n,g_canned_cycle,g98_g99,x_f,y_f,reference_plane,program_block_2,canned_feed_rate

Script Block for program_block_2

2002. Program Block 2. peck drill peck / depths
	DEPTH = MILL_GetDrillDepth()
	PECK = MILL_GetPeckDrillIncrement()
	NUMPECKS = Abs(DEPTH / PECK)
	If NUMPECKS - Int(NUMPECKS) <> 0 Then
		NUMPECKS = 1 + Round(NUMPECKS, 0)
		PECK = Abs(DEPTH / NUMPECKS)
	End If
	CALL MILL_SetReturnString(" I-"&MILL_MakeRealString(PECK)&" J"&(Abs(NUMPECKS)))

If these canned cycles are working correctly then your post could be updated to included these drill cycles and make you one happy man.


To be honest we have all been there, where things don't go right and cost us money. So I understand your frustration and are happy to help. From what I can tell all of your issues should be sorted out based on this thread. CNCZONE is awesome!

Please let me know if there are additional questions or anything else I may be able to help with.