I recently purchased a Emco Compact 5 PC lathe using the Emco software. I need to be able to load the geometry from my AutoCad DXF file but I am having problem viewing the geometry when loaded. It goes through the motions as far as loading and the file shows up but when you open the file nothing shows up in the work space and I am unable to locate it outside of the work space. Are there any tricks to loading or DXF file set ups I need to know about. I will have a machine for sale real soon if I can not figure this out. Thanks!

Any other links where info can be found?

the emco is a nice little lathe, however it does have some quarks with it. I would suggest for getting into it here might not be the best place, but head over to these yahoo groups.

http://finance.groups.yahoo.com/group/emcocompact5users/

you have to sub to read the messages in it but it is definately worth it. I'll try and help out as much as i can with it, but i'm by no means an expert

Thanks but I have already been there with no luck. I am just trying to ask anywhere I can before I decide to sell it.

Thanks again!

silly question here, why do you have to use the emco software? it is very limited and well sucks to be honest in comparison to todays tools. if you have a minute explain what your end game you would like from the emco and i might be able to help out a bit more.

thanks

there is no reason I need to use the Emco software at all. Give me a suggestion of what to use that will allow me to import the AutoCad DXF files into the software and generate the code that will operate the Compact 5PC. I have about 30 DXF files I need to load and DO NOT want to waste my time trying to redraw everything to make it work, at least on the Emco software I do not want to redraw it. If there was software that was easy to draw in like AutoCad I would be fine with that. Thanks!

ok, there is a good and a bad to this. the good is that what you want to do can be done and actually it is pretty easy, the bad is it requires mastercam. currently that is the only program out there that i know of that has a post processor for the emco compact5. i will walk through how i do it and if you want more info because it sounds like it will work for your setup let me know and i can get into more detail. first i use autocad to draw up what i want to cut. after i get it done i then save it as a autocad lite/12 .dxf file. from there i load it into mastercam. I have the emco as my default post for the application. i go to the toolpaths and tell it where to rough and finish and the cutting depts and then i post it out and save it to a file. after that i have my emco connected to my pc and transfer the file over using a program called nclite, i zero out my part then run the program.

if that sounds like it might work for you or whatever let me know and i'll help you out however i can.

later

Sounds like you are doing exactly what i would like to be doing. If you don't mind and when you get time do you thing you could e-mail me with what version of MasterCam (if there are any) you are running or just some specifics so i can try to duplicate what you are doing. My e-mail is grob@htc.net

Thanks!

if you dont mind i would like to post here, i know there are a few others using the emco and if they could benefit from it as well then more power to all of us.


glad to hear i might be of some help too.

all right here is how i do it, btw this is long so sorry :)

first i draw up the part in autocad, actually only the top half seeing it is on a lathe and everything. anyway after i get the part drawn i save it off as a autocad .dxf acad 12/lt file. from there i load up mastercam 9.0 i go to file/converters/autodesk/read file and navigate to the dxf i want to import. that will load up the file.

now i need to post it but there are a few things that need to be done to mastercam, only once, but need to be done anyway. the following is a cut and paste of what you need to do but should get you through it.


----------------------------
Hello everyone, due to the many questions asked about updating MasterCam and
the post that works with the CNC5, I'll give everyone a quick lesson on how to
do so. One warning: If you don't feel confident enough to carry out these
instructions, "DON'T DO IT!!!". Only if you think you can follow these
directions should you try and do so, OK? Good! Now then, the first thing you
should do assuming you don't have the right post processor, is go to the
MasterCam educational division web site and download the post for the Compact 5
CNC lathe. You can go to my web site at:
http://www.angelfire.com/emo2/cnc5doctor for the web link to that site and get
it if you need to. The download will be in the form of a .zip file. If you don't
have WinZip, I have a link at my site that will take you to a place where you
can get a trial version of WinZip free, that will be able to unzip the file to
your computer. The MasterCam post that you want is: "Mplcnc5.pst". Make sure you
get the right post. Now, with post in hand, go to your computer. Click
>"Start" then "Run". Have your floppy disk you zipped the post to in A:\
drive. Type: A:\ in the window, then click the "Browse" button. Click on the
"Mplcnc5.zip" file, then hit "OK". Hit "OK" again. You will be ask where to
unzip the file to. Type in the window: C:\Mcam9\lathe\posts. Then click on
"unzip". This will load the post to the right folder in MasterCam. If you have
another version of MasterCam other than version 9, just replace the number other
than 9, OK? Then the last step is click on "Close". Now, open the MasterCam
program on your computer. Click > "Main Menu". Now hit the "Alt + C" keys
together. This will open the Chooks section. In the window, look for the
"UpdatePST9.dll" file. Click on it to highlight the file, then click on "OK". It
will ask you what file you want to update. Make sure that the post to update is
the "Mplcnc5.pst", then click > "Update". This puts the necessary updates
into the post, if you fail to do this, you will get error messages up the ying
yang. It will ask you if you want to see the updates, either answer yes or no,
depending on how you feel. After all this is done, go back to the main screen.
Now we are going to set the CNC5 post as the default post, and here's how: Click
> "Main Menu" > "Screen" > "Config". You will now be in the
configuration window. You will see tabs towards the upper portion of the window.
Click on the "Files" tab. The window on the right will have post processors
highlighted. If its not highlighted, highlight it. Below that, a small window
saying "Active post" will show the current default post. Click on the box to the
right of that window to open the post processor list. Search and find the
"Mplcnc5.pst" file, click on it to highlight that post, then click "OK". The
active post should say "Mplcnc5.pst". If it does, click "OK" at the bottom of
the window. You will be ask if you want to update the configuration, click >
"Yes". You now have changed the default post to the "Mplcnc5.pst" for the CNC5
lathe!! Now lets update the post for the CNC5. From the "Main Menu" click
>"File" > "Edit" > "PST". You will be asked what post you want to
update. Make sure it says "Mplcnc5.pst", then click "OK". You will see two
windows, make both of them "full screen". You will now see the MasterCam post
processor file for the CNC5. Under the Headline at the top, look for "Revision
Log" just below it. Look for the third (#) sign down. Put your cursor to the
right of it and click to put it there. Then hit "Backspace" on the key board
erasing the (#) sign. Hit the space bar once, the type SEXTNC, hit space bar 5
times, the type, # Use this to remove the file extension , do not put a period
at the end of the line. Next, go down to the "Formulas - Use" section. Look for
the line that says "seqmax : 200". Change this number from 200 to 211. This
gives you a few more lines of code to work with. Now, go to the "Postline"
section farther down the file. Look for the "psof" line, that is the start of
file for non-zero tool n
umber. Put a (#) in front of the line that has the "M06" in it. This will keep
the post from using this line. Now for the last steps, go farther down the file
to the "Numbered questions for MasterCam" section. Put these answers in the
proper question numbers:Question 80 = 2Question 81 = 300Question 82 = OQuestion
83 = 8Question 84 = 1Question 87 = A Once you are done with that, click the "X"
in the upper right hand corner of the "SMALLER" window. MasterCam sees you have
made changes to the post file and want to know if you want to save the changes,
click "YES". Then click the "X" in the "OUTER" window. YOUR DONE!!! Wasn't
that easy?? Go to the main menu and go from there. Hope these directions helps
everyone setting MasterCam to the CNC5. GOOD LUCK!!
-------------------------------------------------

ok, enough of a copy and paste, now that you have the mastercam post you are able to do the fun stuff. ok you have the part loaded up and want to post it. well in mastercam you go to the main menu, then toolpaths, then rough and finish your part off, or just rough it or just finish it whatever you are needing to do, also make sure you are taking off the correct amount per pass. once you get done with this you can go to operations, click on your drawing name and then press the post button to the right, that will bring up a window that will allow you to save the nc code needed to send to the lathe.

now we are almost ready to send to the lathe, first look at your nc file, under the f values i have to add a trailing 0 to my values or else my program doesn't work, depending on your version of the emco you may or may not have to do this. ok now to send it over i'm going to copy and paste from another link and you should be golden at that point.


--------------------------------------------
as for connecting to the compact 5 that
appears to be where you are getting a little hung up. I have not
been able to connect with anything but freenclink and here are the
directions, this should work for any nc linking software, and if you
cant find nclinkfree let me know i'll get it out there somewhere, it
should be available from onecnc, but i can never find it on thier
site.

inside the nc software set it up in this manner
set your com port to whatever one you want to use
baud = 300
data bits 7
parity = even
stop bits = 1
xon/xoff not checked
dtr/dsr not checked
rts/cts not checked

first lines and last lines = 100(0)
i dont know why it's that way but it needs it there
timing line delay (msec) = 0
ignore line prefix = (
add to end of line = "select CR+LF"

ok, now that the options are set how to get the file over there

turn on emco cnc
start nclink free on the computer
on the emco press the "H/C" button
then hit the "inp" button
then type '66'
then "inp" again
a screen should come up rs232 operation etc....
then hit "inp" again
the screen should say load program
now go back to the computer and load up your program
you want to send over in nc link
go to utilities, then send
do not mess with the settings and click on the start button
the emco screen will say "program being loaded" and once done it will
have the program up on the screen
now go over to the emco and hit the start button
-----------------------


good luck and if you have any questions let me know and i'll try and help.

Great stuff! The Mastercam is no problem but what about the linking part of it. Where do I find this?

My compact 5 is the PC so I have a seperate PC for it. I will have only AutoCad, Mastercam and the linking software on it so I can do it all at one PC. i hope this will work.

Thanks!

when you say link are you talking about the serial cable linking the pc to the emco or the software freenclink?

later

The freenclink!

http://www.caddepot.com/cam/NC_LINK.zip

that should be it, gl

Double G, are you making goose calls with this lathe? If so let me know how it's working out. I'm debating on whether or not to get one of these for wood calls.

Well that is the intended use. I was goping to use it for my duck, goose, deer and some call parts but I have to get it where I can load my Cad files. I installed the MasterCam as suggested above and that worked great. now I just need to learn how to use MasterCam and i should be OK. It is actually a real nice little machine but I just need to be able to load my stuff on it.

A quick question about these machines. Can you write and store your programs or do you have to use some sort of a cad/cam package to make parts? Does the machine use standard or close to standard G and M code programing.
Thanks for the help,
Dave

Actually the answer is Yes, Yes and Yes. You can draw your own parts and program from the machine software. Yes you can draw your parts in another program and import the files and program them (this is the problem i am having). And Yes you can use aftermarket software to draw and post your parts to the machine. I have mastercam loaded also but I just need to learn the MasterCam software. Yes it uses standard M and g codes.

Does any 1 know where I can get a wiring Diagram for A Emco compact 5 cnc lather ? I need to fiqure out why I dont have any X or Y movement but the turret moves? X and Y jogs on the screen but the slides and servor mototrs dont move and stay cool while the turret motor get warm which is normal for warm motors... just got this lathe and Im tring to get it to run..

Thanks for any help
Gene

Hi Gene,

Have you joined the Yahoo group for the Emco Compact 5?

http://finance.groups.yahoo.com/group/emcocompact5users/

If you have a look in the files section on that group, there is a service manual for the Compact 5 CNC. I'm not sure if it will have what you need, but it is fairly comprehensive.

Regards
Warren

Hi Gene,

Have you joined the Yahoo group for the Emco Compact 5?

http://finance.groups.yahoo.com/group/emcocompact5users/

If you have a look in the files section on that group, there is a service manual for the Compact 5 CNC. I'm not sure if it will have what you need, but it is fairly comprehensive.

Regards
Warren
thanks Ill try there

my problem is more severe i cant end my program on my cnc5 I put a g22 code in and get a A00 error? Any ideas
Thanks
Gene

I also have a CNC5 and have been having some difficulty with using MasterCAM to generate good code. I made the changes and updated the post as you suggested but still am having alarm problems with GO2's 3's. I can run a program and it will go through a couple 02 03 with problem then come to one and get the wrong radius alarm. Sometimes it won't even put a circular movement where there should be one. Do you have any other tips that might help?

Also, to Double G, I was having the same trouble finding my drawing when using a dxf and it was being loaded in the lower left of the screen view. So I did my drawing in the upper right and was able to find the drawing and then shift it into place.

thanks Ill try there
Do you know of a diagram for a compact5 PC machine?

I have a emco cnc 5 and am using mastercam with the post update as shown in H2O's thread, but still can't get the thing to work right. If there is anyone successfully using the cnc 5 and mastercam could I contact you to talk about mine? I have worked with mastercam getting this to work right but they don't seem to really care a whole lot. I would just like to see how your config settings and other parameter setting are set up.

i have a good working post for mastercam 9 if anyone needs it let me know how to put it on here and i will i have ran several parts with it and it is working fine
joe

Im new here, new to cnc, and pretty new to lathes:P I need the manuals, programs, and to know how the computer hooks up. The machine has no paperwork and there is 1 connector not being used on the back of the lathe but no more cables. I checked the yahoo group but the cnc manual was a link which is now dead. I don't know what mastercam is other than checking their site, and I don't have the post processor either.

Any help is greatly appreciated. I can get help with the lathe itself but making it communicate with a PC, and then taking autocad files and converting them is what I will probably be hung up on.

You guys with the compact 5 lathes might want to look at the welsoft upgrade for these lathes, go to www.welsoft.com thay are in the UK.

Hello,

what is your EMCO Compact 5 PC Software Version?

regards

Frank

Does any 1 know where I can get a wiring Diagram for A Emco compact 5 cnc lather ? I need to fiqure out why I dont have any X or Y movement but the turret moves? X and Y jogs on the screen but the slides and servor mototrs dont move and stay cool while the turret motor get warm which is normal for warm motors... just got this lathe and Im tring to get it to run..

Thanks for any help
Gene


Gene,

I wonder if you managed to get a schematic? I am now in a similar situation and wonder if anyone can help. I purchased a compact 5 with turret a few weeks ago and have so far played around and turned out a few simple parts, I seem to of caught the bug though because I got a follow on from a guy with a later model compact 5 with M codes offering me a complete faulty machine with spares including chucks and a milling head. Apparently the spindle turns but there is no x-y movement and he has been told it is probably a relay fault.

So I am on the lookout for some info, unfortunately the Yahoo group link in this discussion seems to be inactive now.

Any help from anyone would be greatly appreciated.

Kevin

here you are gents here is a valid link for that emco user group. ive got all the files for the manual which include a simple wiring diagram which does display stepper motors connections etc, use that link or if still having trouble p.m your email me i'll mail the files over

hello gents, here is a valid link for that yahoo user group:

http://finance.groups.yahoo.com/group/Emco_cnc_users/

if anyone is still having trouble getting the manual p.m me i can send it over through email i have saved it onto hdd.

there is a wiring diagram on page 35 perhaps it will help some, im not sure it is the full diagram for the machine just the main connections between hardware.

I'm just curious.
Would it be worthwhile and worth the $ to update the drivers/ boards (but keep the motors) to something capable of running something more current like Mach3 etc.? I'm in the process of updating a bridgeport type mill and it's not all that expensive. I would think that for under $500 or so it should be doable and might give you much greater flexibility.

Just a thought...

Hello,

i have designed a Interface Kit for EMCO Compact 5 CNC & 5 PC to use all
Software with Step/Dir. Use also original Encoder. Can switch between Full
Step / Half Step. Only move out CPU Board and Plug in the Interface.
The price for the Interface is Euro 400,--. You can see it on my Homepage
www.scnct.de But it´s only in German Language in the moment.

regards

Frank

First you have to understand where the position of the part is on the screen vs. when you open it up in another software package. to make it easy make a simple box drawing on the EMCO screen and save it in the "Archives" as a drawing (.dxf) file. Then open the desired CAD program and it will be in the upper +y,+x quadrant, note the position in X & Y and you can make yor drawings in this location, this way they will be in the correct area when you load them into the EMCO software. Any drawings drawn & saved in the EMCO software will load up in this area.
Once you "think" like the software its pretty simple. I make my drawings in the EMCO software and have been able to open them in BobCad, MasterCam, etc. I use the EMCO software to generate he code as well, sometimes its quirky but I have made dozens & dozens of parts on my PC5.
Do you have the EMCO manuals for programming?? They are much easier than AutoCad to learn as they were designed for highschool students with no expirence.

The motors are the first thing I would toss. They are like 60 oz inches and the resolution is about 1\3 of a modern 200 step motor. These motors are no longer avaliable and when they were were outrageously expensive at $ 500.00 EACH!! EMCO didnt use off the shelf motors and these were custom made for them.
First thing I would do is get 2 nice 145 oz. Pac Scientific steppers, drill & ream the shaft for the pin for the cogged belts, get 2 Gecko drives, breakout board & power supply. Mach3 software and your done, about $ 800.00.
A local engneer is working on a custom turret for these series lathes (PC5) as they werent offered with one from EMCO.

Did you check the fuses?, if you have no X or Y movement your stepper motor board may be bad, they can self desruct like mine did. Usuallywhen this happens the steppers go out as well. I have a CNC5 and one night afer work I decided to run a few parts, switched on the lathe and ran a program. About 15 seconds later I noticed the slides werent moving and I sawa perfect colunm of smoke rising about 2 feet over the "Z" axis. First reaction was "cool !!" but then realized it had taken big dump on me !! I called EMCO and almost fainted when they told me the price of the motors & stepper board. I found a good deal on the PC5 and am finishing up the conversion of the CNC soon.

Hi All...

I just discovered the CNCzone and it is great... I have a CNC5 that has had the electronics poop out... Or at least I think so. The tape drive had a problem, so at the suggestion of a gentlemen on the Yahoo users group, I just un plugged the drive and entered a short program by hand. It worked as fine... After not using the lathe for a number of months, I tried it again and now it won't work at all... The little 1 amp fuse on the power supply pops as soon as I turn on the power... Oh well, time for a retrofit I suppose...

Do any of you gentlemen have any suggestions for an idiot proof, bolt on, 'plug-n-play' retrofit system? Or how about a website that may offer such a system?

I would like to get the lathe working again...

Regards
and Happy New Year to you all...

Bob Emott
birtyres@nsm.com

Bob,

I am retrofitting a Compact 5 PC lathe and have an available stepper board and original stepper mottors if you are interested. The Compact 5 PC and Compact 5 CNC use many of the same boards.

The part number on the stepper motor board I have is:

A6C403000
A6PC-001/U4

Look up the part number on your board and if the same this one may be of use to you.

If interested we can discuss how to trade. I would consider selling or trading for tooling.

Ed

Thanks for the offer but I think I want to do a complete electronic retrofit of my lathe. I had already purchased a new tape drive to try to get my lathe back into operation and this swap was not sucessful... So I think a complete changeover is my best route...

I tried the emulate this but i can only download a program from my CNC5 for some reason I cannot get the upload to work. I really do not understand this part:

first lines and last lines = 100(0)
add to end of line = "select CR+LF"

Did you actually type in "select CR+LF" with quotes and all? I tried that plus just using ascii keys and still did not work.

Any insight would be helpful.

Dan



all right here is how i do it, btw this is long so sorry :)
--------------------------------------------
as for connecting to the compact 5 that
appears to be where you are getting a little hung up. I have not
been able to connect with anything but freenclink and here are the
directions, this should work for any nc linking software, and if you
cant find nclinkfree let me know i'll get it out there somewhere, it
should be available from onecnc, but i can never find it on thier
site.

inside the nc software set it up in this manner
set your com port to whatever one you want to use
baud = 300
data bits 7
parity = even
stop bits = 1
xon/xoff not checked
dtr/dsr not checked
rts/cts not checked

first lines and last lines = 100(0)
i dont know why it's that way but it needs it there
timing line delay (msec) = 0
ignore line prefix = (
add to end of line = "select CR+LF"

ok, now that the options are set how to get the file over there

turn on emco cnc
start nclink free on the computer
on the emco press the "H/C" button
then hit the "inp" button
then type '66'
then "inp" again
a screen should come up rs232 operation etc....
then hit "inp" again
the screen should say load program
now go back to the computer and load up your program
you want to send over in nc link
go to utilities, then send
do not mess with the settings and click on the start button
the emco screen will say "program being loaded" and once done it will
have the program up on the screen
now go over to the emco and hit the start button
-----------------------


good luck and if you have any questions let me know and i'll try and help.

Bob,

I am retrofitting a Compact 5 PC lathe and have an available stepper board and original stepper mottors if you are interested. The Compact 5 PC and Compact 5 CNC use many of the same boards.

The part number on the stepper motor board I have is:

A6C403000
A6PC-001/U4

Look up the part number on your board and if the same this one may be of use to you.

If interested we can discuss how to trade. I would consider selling or trading for tooling.

Ed


Still have any parts available? I'm looking for a CPU board part number A6C114004 to upgrade my A6C114003.