Emco Compact 5 PC...have ????

[Double G]

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?

[h_2_o]

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/grou...compact5users/

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

[Double G]

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!

[h_2_o]

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

[Double G]

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!

[h_2_o]

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

[Double G]

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!

[h_2_o]

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.

[h_2_o]

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.

[Double G]

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!

[h_2_o]

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

later

[Double G]

The freenclink!