[Clarke Yeager]

I Need Help!I recently purchased a Bridgeport R2E3 series II milling machine for my home shop. I purchased a Operating Manual and a Boss 8 R2E3 Programming manual. I spent a lot of time getting it up and running, but finally succeeded. I have FeatureMILL program to design my parts in and a ConnectCNC program to send programs to the mill. FeatureMill does not have a post for a BOSS8 machine but I can set my machine to accept BOSS 4-7 data. I can down load programs to the mill using ConnectCNC through the port B RS232 port. This machine only has 2K of memory, EXTREEMLY limited! Both the mill and the ConnectCNC program are capable of Drip Feed DNC but I have not been successful at getting it to work. I have tried many configuration setups but I constantly get an error code of 0040 (communication error). Can anyone out there help me getting my machine to accept Drip Feed?Clarke Yeager

[machintek]

Not too long ago FeatureCAM came with EZUTLS for communication with a Bridgeport. This included EZLINK for communication through port B.
The BOSS 8 and 9 posts were identical and were also included. Call them if you do not have these posts. They should be available.
I used EZCAM on a MAC with my BOSS 9 but always modified my programs using loops and macros for multi-part fixtures (no 3D stuff) and could take a 8 page EZCAM program and condense it into less than a page. Most posts spit out a lot of repetitive unnecessary stuff.
I hope someone answers that has actually DNCed to a BOSS 8.

George

[Jim Bass]

Hi Clarke,
I may be able to help you, I use FeatureCam ver.7 with a BOSS8 series I.

1 - What version of FeatureCam do you have?

2 - Have you found EZUTLS that George Suggested?

3 - What are you using for a computer to download to the BOSS 8 controller?

If we work with EZLINK, BOSS 8 and FeatureCam I will try to help.



FeatureCam ver.7 has a post processor for BOSS 8.

Look in the FeatureCam directories, should be one named EZ-Utils. Run that program. The one with ver.7 brings up a screen named EZ-Utils 6.2.1. You have tree choices: To CNC -- From CNC -- Setting . Start with settings, you will need to set both EZ-Utils and the BOSS 8 controller to the proper parameters (both must be the same).
BAUD rate should be 4800, nothing else. The BOSS 8 controller may need other setting as for proper communication.

You will also need to set the directory from where EZ- Utils will find the program you wish it to load. I have a directory that I have named cncdump that I copy my cnc programs into and EZ-Utils is set to look in it for program to load.

Post again after you have worked through the above and we can go from there. The set up of the Bridgeport CNC’s can be a pain, but once done your set to go from there on.

Jim

[Clarke Yeager]

Thanks so much to both George and Jim for responding and trying to help me. You guys are great!

I didn’t realize that EZ-UTILS was included in FeatureCam, I was trying to find it as a separate program. I also set FeatureCam to BOSS8 post. I have EZ-UTILS working fine for transferring small CNC programs to the Bridgeport mill memory.

I still am having problems with DNC drip feed. The drip feed seems to be working in the since that I can run programs from my PC now in drip feed, but they don’t run correctly. A program I tried cuts a circular pocket. It ramps down a little then cuts a circle. It ramps down a little more and again cuts a circle. FeatureCam spit out a program that has a sub routine to cut the circle after each ramp down.

I made it a small program so I could run it both from memory and from DNC to get a comparison of how it works. When running from memory, it works fine. When running from DNC link it doesn’t like the sub routine, it stops after the first circular cut with what I believe is EOT. Below is an example of a simple round pocket that uses a sub routine that doesn’t run with DNC but runs fine from memory.

If you know any solution for this problem I would appreciate it!

Answers to your question Jim:
1) My FeatureCam version is V13.1.0.28
2) I did find EZ-UTIL and it is functioning for small files
3) I am using a DELL lap top running XP. It doesn’t have a serial port so I am using a USB to serial converter which looks like com3 to the computer.

Thanks
Clarke


.N10G70G75G90
'Tool Stand 4 hole small 6-9-2009'
'POCKET2'
'TOOL NUMBER:1 SPINDLE RPM:3972'
N30G0X0.Y0.T1M6
N35X-5.5231Y-2.6519
N40Z0.1M8
N45G1Z0.01F29.8
N50X-4.9819Y-2.3394Z-0.035
N55X-5.5231Y-2.6519Z-0.08
N60X-4.9819Y-2.3394Z-0.125
N65X-5.2525Y-2.4957F99.3
#1
N75G3X-5.2525Y-2.4957I-5.25J-2.5F99.3
N80G2X-5.2916Y-2.428I-5.272J-2.4618
N85G3X-5.3306Y-2.3604I-5.3111J-2.3942
N90G3X-5.2121Y-2.3433I-5.25J-2.5
N95G2X-5.3556Y-2.2839I-5.0938J-1.8546
N100G3X-5.5078Y-2.3147I-5.4151J-2.3814
N105G3X-5.5078Y-2.3147I-5.25J-2.5
$
=#1
N120G1X-5.5231Y-2.6519
N125X-4.9819Y-2.3394Z-0.16F29.8
N130X-5.5231Y-2.6519Z-0.205
N135X-4.9819Y-2.3394Z-0.25
N140X-5.2525Y-2.4957F99.3
=#1
N150G1X-5.5231Y-2.6519
N155X-4.9819Y-2.3394Z-0.285F29.8
N160X-5.5231Y-2.6519Z-0.33
N165X-4.9819Y-2.3394Z-0.375
N170X-5.2525Y-2.4957F99.3
=#1
N180G1
'POCKET2'
.N190F99.3
N195X-5.5498Y-2.3564F78.0
N200G3X-5.5752Y-2.4098I-5.4096J-2.4558F39.0
N205G3X-5.5752Y-2.4098I-5.25J-2.5F40.5
N210G3X-5.5874Y-2.5087I-5.25J-2.5
N215G3X-5.5757Y-2.5668I-5.4156J-2.5043F39.0
N220G1X-5.545Y-2.6174F78.0
N225G0Z1.0
N230X0.Y0.M2

[machintek]

Two possibilities.
First timing issues with the USB to COM port converter. I say this because I installed a servo driven auto door on a CNC lathe and it drove me crazy trying to communicate with the unit the same way. once I found a PC running XP with a com port, all was well.
2nd thought and the most likely. In DNC, the control takes one line of data at a time, and has one in a buffer, thus if you specify macros and call them up, it cannot go back to see them. If the complete program is in memory and DNC is not used it can access whatever part of the program it needs.
Try reposting with out macros, and DNC that.

George

[Clarke Yeager]

Good morning George,

Thanks for the information. I obviously don’t have much time working with drip feed but
as far as I can tell all functions other than sub routines seem to be working. I don’t know about loops yet however and may have other issues that I am unaware of. The machine supposedly is designed to works with drip feed and I would think that it has some means of doing sub routines which are heavily used in programming, both written and generated from CAM programs.

Timing is a real possibility because of using the USB to serial converter, especially since you had similar problems when you used one and it worked using a machine that had a serial port. I will have to see if I can find a computer that has a serial port. Right now I don’t have any access to one.

Thanks,

Clarke

[Clarke Yeager]

George,I think you are probably correct when you say Sub routines don't work because they don't reside in memory. I believe a simple solution for this is to modify the program and every where there is a call to sub routine just copy the sub routine to that point and eliminate the call. I have not tried this yet but I believe it will work and is a simple fix for the problem.Thanks so much to both you and Jim for all of the help. Your help has helped me gut up and running!!Best wishes to both,Clarke

[machintek]

Since my answer, I did talk to a very old wise friend (not old in age) who told me the same thing. No macros or loops in DNC. Those are used to make a program smaller to fit in the limited memory of these old controls. If you DNC, it is irrelevant to make the program condensed.
Glad I could help.

George

[jp86cj7]

I have a 1984 Bridgeport R2E3 Series I CNC Milling Machine (Boss 8).
Could someone tell me where I need to look for the Serial Port connection.
I would like to connect my PC to it and use Hyperterminal to control it.

Does anyone have any manuals and could tell me on to program it?
Is it just G-Code to control it?

Thanks
Jay [email protected]

[MrBoss8]

Clarke, Machintek hit the nail on the head. The beauty of DNC is who cares how big the file is, no worries! And may I ask how you know you have only 2k memory? I thought all R2E3's had about 11K. My machine has successfully loaded 11,970 char. before I receive a communication error.

Hope its coming together for you.

[Neal.R2E3]

I just bought a r2e3 in great shape and I'm using mach 3 conversational and lazycam to generate g code and oneCNC NClink to send the g code but the rs 232 cable got cut in half when I was loading up the machine does anyone know how to wire up a new one and does anyone have access to r2e3 boss 8 owners manuals and or proggraming manuals or where I might purchace them from. I finaly ran into something I can't find on the net.

[machintek]

If the cable got cut peel it back and solder it back together.
There are only 3 wires that communicate and should be color coded.
Transmit, receive, and signal ground.
Typically, pins 2 and 3 are transmit and receive (or visa/versa, if a DTE or DCE) on a DB25 and 7 is signal ground. There are 2 jumpers on the PC side: 4 to 5, and 6 to 8 to 20.

George

[Neal.R2E3]

the cable was cut be the shop owner still has the computer end.