[Bill Gillen]

Hi,

We wanted to ask how do you make a Bridgeport R2E3 mill execute nc code, once it is loaded into the original Bridgeport controls? We have read the operator's manual several times, and just haven't figured out how to put together the correct sequence of operations to make chips.

Does anyone know the correct sequence of button pushes on the control to make the mill able to execute the code? Right now we just want to make sure we can make it work, and then we will start creating parts, or at least putting workpieces in harm's way : ).


A little background:
Over the past few days, weeks, we figured out how to load nc files to the Bridgeport R2E3, equipped with original Boss 8I controls. The NC code was developed by ONECNC XR, using the Boss 9 post (next choice is Boss 6). We strip the .nc off the end of the file name before transmitting it via NCNet Lite (the free stuff) over a special serial cable into Port B.

We can verify the code is in the Bridgeport controls by using Find, and then selecting any N number (like N100) to see the code, which matches the NC file. Now we're stuck, but realize we're still newbies trying to muddle our way through something new to both of us.

Thank you,
Bill Gillen and Tim Glover

[HuFlungDung]

What messages does the machine give you on startup? Does it require that you home all the axis (to some homing switches) before it says it is ready?
If you have a program in machine memory, it should be ready to run, but as a precaution, it is always a good idea to not have any tools in the spindle at this point, and have the knee lowered as far down out of harm's way, as you possibly can.

Somewhere on the operator panel, there should be a knob, with a "mem" setting. Perhaps another knob with "Single" and "Auto" etc. I have never seen one of these, so I don't know what the operator panel looks like.

Anyway, here is your thread bump

[Jim Bass]

Hi Bill & Tim,

From your post I'm guessing you have a BOSS 8.

First you need to press "Axis drive enable" ( that will home you machine)

Next press "Reset program"
To run program -
Press "Auto
Then "Start" (Machine will travel to 0/0 and stop, looking for tool change, insert tool # 1, make sure you have set tool lengths)
Turn spindle knob to "High gear" and press "Spindle enable" at the same time, program should run.

You may have trouble using the BOSS 9 post, check with CAD/CAM mfg to see if they have a post for the BOSS 8.

Yours, Jim

[Jim Bass]

Hi Guys,

Forgot one step, press "Start" again, then program should run.

Jim

[Bill Gillen]

Thank you for the tips. We will try this at lunch today. Have to take care of the day jobs first . We have the table lowered waaaay down, as we don't want any crashes.

Tim Glover and Bill Gillen

[machintek]

Just a note, you MAY need to find a program if it starts with a valid Bridgeport BOSS 8 name. Example of a valid program name starts with a colon and has a number (:3004).
Then you can run it. The BOSS 8 differed from the previous BOSS machine in that it could store more than one program thus the need for program numbers. BUT the programs had to end with a M30 to rewind the program being used. If a Mo2 was used it went to the first program in memory.
Did you check with www.machinemanuals.net for a operating manual on CDROM? Or Ebay?

George

[Bill Gillen]

Hi,

Thank you for all the suggestions so far. We feel like we are definitely making progress. We followed Jim and George's suggestions, and it works fine up to the point it is supposed to execute the program. Following is what the readout shows just prior to trying to execute the program:

N0 T01 SF
then we see
N20 (FILE - C:\ONECN..... (which is what is in the file)
then we hit START and
N30 T00 SF pops up on the readout (this is not in our file)

After we hit start again, it stops the spindle, the Program Stop LED comes on, and it jumps back to N20.

We haven't had any success getting past this point. We just made a quick program (is part of a hamburger patty making plate) to see if everything functions from the CAM program to the chipmaking. I am enclosing the latest iteration. Per George's suggestion, I changed the file number in the NC file from o0000 to :0012. We realize we may have a post problem (OneCNC XR does not have any posts between Boss 6 and Boss 9.

The readout on the mill says Boss 81 I.

I figured it is safer to assume at this time our lack of knowledge is more of a problem than the software : ).

Here is the latest program we tried:

%
:0012
N10 (PART - )
N20 (FILE - C:\ONECNC-XR\MILL ADVANTAGE\XFA\FOOKS.XFA)
N30 (AUTHOR - DEFAULT)
N40 (GROUP - TOOLPATH GROUP #1)
N50 (POSTED - TUESDAY, MAY 31, 2005 13:00)
N60 (CREATED - THURSDAY, MAY 26, 2005 15:07)
N70 (SYSTEM- ONECNC-XR MILL ADVANTAGE - VERSION 6.38)
N80 (NOTES - NONE)
N90 G00 G40 G49 G80
N100 G00 G90 G54
N110 M05 G40 G49 G80
N120 M09
N130 (.75 INCH 3/4 HSS END MILL)
N140 T01 G43 H0 D0
N150 M06
N160 F1.02 S300
N170 M03
N180 G00 X2.9836 Y1.8757 Z1.
N190 Z0.95
N200 G01 Z0.25 F0.51
N210 X3.125 Y2.0172 F1.02
N220 Y4.
N230 G03 X1. Y6.125 I1. J4.
N240 G01 X0.5
N250 G03 X0.375 Y6. I0.5 J6.
N260 G01 Y0.5
N270 G03 X0.5 Y0.375 I0.5 J0.5
N280 G01 X3.
N290 G03 X3.125 Y0.5 I3. J0.5
N300 G01 Y2.0172
N310 X2.9836 Y2.1586
N320 G00 Z1.
N330 Y1.8757
N340 Z0.7
N350 G01 Z0. F0.51
N360 X3.125 Y2.0172 F1.02
N370 Y4.
N380 G03 X1. Y6.125 I1. J4.
N390 G01 X0.5
N400 G03 X0.375 Y6. I0.5 J6.
N410 G01 Y0.5
N420 G03 X0.5 Y0.375 I0.5 J0.5
N430 G01 X3.
N440 G03 X3.125 Y0.5 I3. J0.5
N450 G01 Y2.0172
N460 X2.9836 Y2.1586
N470 G00 Z1.
N480 (END TOOL)
N490 M09
N500 G91 G28 Z0.
N510 G91 G28 X0. Y0. M05
N520 M30
%


Any more suggestions?

Thank you,
Tim Glover

[Bill Gillen]

Does anyone have a sample nc file (small one is fine, but we will be glad to accept anything) written for the the Boss 8 control they could post here? I talked to Val at tech support for One CNC, and he is probably going to write a new post, but is looking for samples to work from. Obviously, I don't have any good ones yet. They have Boss 6 and Boss 9 posts, but nothing in between.

Thank you,
Tim Glover and Bill Gillen

[Jim Bass]

Hi Bill,

George is right, you need to have a program name for the BOSS 8 file, as he stated the control can hold more than one program. The control will hold up to 12,000 characters in the text buffers.

The post you are using may be a large part of your problems. Look at the sample I posted. You will see that it uses G0, not G00, The manual states "G code consist of address G plus up to 3-digits and specify various control modes", but all the examples listed in the manual consist of G0, G1, G90, G70 and so forth. They never use G00, G01, G001, G090, or G070. Go figure???
They do not show three digit numbers until they get to canned cycles, such as G172 pocket frame mill.

The manual I have for the BOSS 8 states that you need to name the file with a five digit number, with the first valid number being 15000 The file ends with a .txt extension.

This program was wrote with FeatureMill cam software. You will need to put the following text into a file named 17006.txt Load program by entering 17006 when control calls for program name. It uses one tool only, so make sure you have set the tol for tool # 1


.N10G70G75G90
'Printer Roll Removal Tool 6-4-2005'
'BOSS1'
'TOOL NUMBER:1 SPINDLE RPM:2800'
N30G0X0.Y0.T1M6
N35X-9.5Y-3.0
N40Z0.1M8
N45G1Z-0.2175F10.0
#1
N55X-9.1339Y-2.265F20.0
N60G17G3X-9.156Y-2.0486I-9.2704J-2.1696
N65G2X-9.2813Y-1.7509I-8.8813J-1.7579
N70G1X-9.2704Y-1.126
N75G2X-7.719Y0.3722I-7.7456J-1.1526
N80G1X-6.7415Y0.3551
N85G2X-5.7037Y-0.0471I-6.7696J-1.2576
N90G3X-4.9959Y-0.3214I-4.9767J0.7784
N95G2X-4.9935Y-0.3215I-5.0007J-0.5964
N100G1X6.6781Y-0.6293
N105G2X8.0082Y-1.0885I6.6371J-2.9039
N110G3X8.3561Y-0.9837I8.1438J-0.9089
N115G2X8.8124Y-0.6665I8.8041J-1.1414
N120G1X8.8154Y-0.6666
N125G2X9.2821Y-1.1498I8.8071J-1.1415
N130G2X8.1122Y-2.2795I8.1322J-1.1297
N135G1X7.6122Y-2.2708
N140G2X7.3533Y-2.2366I7.6323J-1.121
N145G3X6.9307Y-2.1851I6.9349J-3.9101
N150G1X-5.5805Y-2.2155
N155G2X-5.586Y-2.2155I-5.5812J-1.9405
N160G2X-6.5515Y-1.6582I-5.5659J-1.0656
N165G3X-8.4175Y-1.8432I-7.4407J-2.1928
N170G2X-8.873Y-2.1581I-8.8647J-1.6832
N175G1X-8.8883Y-2.1578
N180G2X-9.156Y-2.0486I-8.8813J-1.7579
$
=#1
N195G1X-9.5Y-3.0
N200Z-0.435F10.0
=#1
N210G1X-9.5Y-3.0
N215Z-0.6525F10.0
=#1
N225G1X-9.5Y-3.0
N230Z-0.87F10.0
=#1
N240G1X-9.1647Y-2.0133F25.0
N245G3X-9.1824Y-1.9815I-9.2927J-2.0635
N250G2X-9.2563Y-1.7513I-8.8813J-1.7579
N255G1X-9.2454Y-1.1264
N260G2X-7.7194Y0.3472I-7.7456J-1.1526
N265G1X-6.7419Y0.3301
N270G2X-5.7202Y-0.0659I-6.7696J-1.2576
N275G3X-4.9963Y-0.3464I-4.9767J0.7784
N280G2X-4.9941Y-0.3464I-5.0007J-0.5964
N285G1X6.6775Y-0.6542
N290G2X7.9932Y-1.1084I6.6371J-2.9039
N295G3X8.3796Y-0.992I8.1438J-0.9089
N300G2X8.8119Y-0.6915I8.8041J-1.1414
N305G1X8.815Y-0.6916
N310G2X9.2571Y-1.1493I8.8071J-1.1415
N315G2X8.1126Y-2.2545I8.1322J-1.1297
N320G1X7.6127Y-2.2458
N325G2X7.3594Y-2.2124I7.6323J-1.121
N330G3X6.9306Y-2.1601I6.9349J-3.9101
N335G1X-5.5806Y-2.1905
N340G2X-5.5856Y-2.1905I-5.5812J-1.9405
N345G2X-6.5301Y-1.6453I-5.5659J-1.0656
N350G3X-8.441Y-1.8348I-7.4407J-2.1928
N355G2X-8.8726Y-2.1331I-8.8647J-1.6832
N360G1X-8.8879Y-2.1328
N365G2X-9.2563Y-1.7513I-8.8813J-1.7579
N370G1X-9.2559Y-1.7334
N375G3X-9.2601Y-1.6972I-9.3934J-1.731
N380G1X-9.2736Y-1.6635
N385G0Z0.5
N390X0.Y0.M2


Good Luck and let me know how it works. [email protected]

Yours, Jim

[machintek]

The parenthesis will kill you!!
I believe the BOSS 8 and 9 used single quotation marks that allowed what was between them to be displayed but not be considered part of the program.
Strip them out and see what happens.
Note that it will do rapid moves (G0 is fine) with the spindle off but will halt at a G1 if the spindle is not on.
The beginning should have a tool call (T1M6) to make sure that the correct TLO is being used by the control. If you start the spindle before the tool call it will stop for the tool change and you will have to restart it (hold the forward/reverse to the correct direction and do a spindle enable).
I begin each part of the program (and the beginning) with a safety line that makes sure it is in rapid, in inch, in x/y circular interpolation plane and to make sure cutter comp is OFF. That way if I stop a program and restart it, i do not mess up the cutter comp etc.

George

[Bill Gillen]

Thank you all for the suggestions. OneCNC is currently preparing a post, but it is not quite there yet. In time. Over the weekend, Bill found a Mastercam post for a Boss 9 controller on FastechInc's website, and after changing X60 and Y48 to X5 and Y4, the program appears to execute properly. We are having fun learning, and know eventually that we will "get it" and start making chips.


N100 G75 G90
N102 G0 X5. Y4. T1 M06
N104 G0 X-.25 Y-.5 S1781 M03
N106 G0 Z.25
N108 G0 Z.1
N110 G1 Z-.25 F6.4
N112 Y0. F24.4
N114 Y3.
N116 G2 X1. Y4.25 I1. J3.
N118 G1 X4.
N120 G2 X4.25 Y4. I4. J4.
N122 G1 Y1.
N124 G2 X3. Y-.25 I3. J1.
N126 G1 X0.
N128 G2 X-.25 Y0. I0. J0.
N130 G1 X-1.25
N132 Z-.15 F6.4
N134 G0 Z.25
N136 G00 X5. Y4.
N138 S400
N140 G0 X1. Y3.
N142 G0 Z.1
N144 G81 X1. Y3. Z.35 F4.0
N146 X3. Y1.
N148 G80
N150 G83 X1. Y3. Z.35 Z.1 Z.1 F4.0
N152 X3. Y1.
N154 G80
N156 G00 X5. Y4. T3 M6
N158 S3667
N160 G0 X1. Y3.
N162 G0 Z.1
N164 G84 X1. Y3. Z.35 F183.4
N166 X3. Y1.
N168 G80
N170 G00 X5. Y4. M2