[fitzpatrick2362]

I am currently using Edgecam CAD/CAM software.

I am having trouble getting the correct output on my Maho Post processor.

It is a 3 axis Vertical Maching Centre using Philips control.

Common problems are that Y axis is Z and Z is Y, X+ is X-and various others.

Does anyone have experience with this control or even better does anyone have this post.

[smoregrava]

Hi I'm working on a post for this. I belive that I have this finnished during this summer. I resently bougth a Maho mh500 c 432 controller and I have made the connection to my computer. This works nice. I would love to dripfeed but seems that this is not possible on my control early maho 432 control. I have buildt some postprosessors at my work and have started the prosess with the maho post. I have not tested anything yet but the problem that Y is Z and so on seems to be solved. I will share the post as soon I have something I have tested.

[fitzpatrick2362]

That would be great.

Any help would be appreciated.

[smoregrava]

I have now done the first sucsessful testing with my new post. It now works nice in profiles Axes and radiuses Works. Needs to test some drilling and some 3D motions. I send the post to you as fast I have tested this.

I was fun to se the machine moving along the path I programed in Edge Cam.

[fitzpatrick2362]

Good stuff.

I have not had time to even look at the post lately.

[parveenk78]

dear sir.
i have one maho50 horizontal machining centre with philips432 cnc control but i can't download the programs to my pc i mean i need the wire detail for RS232 communication if you have then please send it to me at my yahoo i d it's [email protected] i will b thankfull for the same
thax
Parveen from india

[smoregrava]

Yes I have what you need to connect and download programs. I wrote this in another thread here at CNCZone
http://www.cnczone.com/forums/showth...t=38719&page=5

But I repeat it here.
I made my Maho 432 to talked to my computer(DNC). I have made a DB9 to DB25 full handshake cable (Like in the picture). And i used Hypertermial to transfere the programs. easy and seems to work nice

Here is how I did it if anyone wants to know:

First I checked Machine constants
Nr 115 =1 means 2 as stop bit (=0 means 1 is stop bit)
Nr 116 Input Baudrate and
Nr 117 output baudrate. In my case baudrate was set to 300, but I found in some papers that they had used 4800 before on my machine so I will change this as soon as possible.

Then I opened Hyperterminal (Is in windows under comunication)

I used this parameters
connect to Com1
Baudrate= 300
Data bits= 7
Parity= Equal
stop bits= 2
Flow controll Hardware

Send CR at line end
Local ecco

Then I go to the controll and press
"MANUAL"
"PART PROG"
I selected ALL MEMORY
press "MEM LOCK"
"DATA INPUT"

Then I used a simple program as a test

% PM
N9008
N1 G1 X20 F500
N2 G1 Y20
N3 M30


I marked the text/program above and rigth click in Hyper terminal window and choose "Paste to Host"

When all lines was sent I have to press
"CTRL+D" on the computer. Then the program is in the controll.
I Actually don't anderstand why I have to press ctrl+D. But its works

I also loaded programs and tool table out of the machine to the computer.

Hope this helps

[parveenk78]

Dear sir..
Thax a lot for helping me i will try the same but i m not able to read this format of wire layout (connection detail for cable) coz it's too small ..can you send it to me with any inlarge view so that i can read the same please convert it in to ms word if u can ..
it will be gret help of mine..
Thax & Regards
Parveen

[smoregrava]

Ok try this. I made the full handshake DB9-DB25. I have this PDF At second page you find the cable info

[parveenk78]

thax a lot for helping me i will try the same and will reply to you.
Thax Again
Take care
Parveen

[parveenk78]

Dear Sir,

i tried the way you told me about but i m not able to download the programe from machine to my pc and not able to upload the programe from my pc to machine basicly we bought this second hand machine and now after a long time it's start we did not run this machine i don;t know about the history of this machine may be there is any other problm with system or any kind of cable i mean to say internal problm in the control..
what do you think about this matter..

i m really thankful of you for spending some time on me if you can guide me more you have any other guidence about this matter then i will b thank full for this ..

Thax & Regards
Parveen from india

[smoregrava]

Are you able to start you machine and use? The machine has to be in manual and the Hyrdaulics has to be active when you send and recive data. This means that the machine can't have active alarms before you transmitt data.
If the machine does start check this thread for more info on startup http://www.cnczone.com/forums/showth...t=38719&page=5

Do you get an alarm when you transmitt data?

[smoregrava]

Here is the post for edgecam:banana:

And I have made a small webside to collect some info on cable, M and G code lists and more. The Edgecam postprosessor is at the bottom

http://smoregrava.net/Maho/mahomh500.htm

Remeber you use this post completly on your own risk. I have made this post for fun and have not tested everything.

If you discover bugs inform me and I'll try to correct it and create a better bug :-)

[parveenk78]

Dear sir.
thax for help me a lot
now days i can down load the progarms from mc to pc but i m not able to upload the programs from pc to mc and machine is misbehaving in this process somtimes no any line goes in to the m/c some times 8 blocks goes in to the mc and som times whole data can be upload but i don't know why this machine is behaving as like this we chekd all the joints and card of machine also. but the problm is still here. somtimes error D32 apears and somtimes error D42 apears on the monitor of machine . please guide me if you can about the same ..and i m using VISI cam for modelling and programming but i don't have the post processor for philips432 ..if you have some link about this post processor then please send me as soon as possible.. i will be thank full for the same..
Thax & regards
Parveen Kumar

[smoregrava]

D32 Is Parity error
D42 Is Baudrate error

So here there is something with your parameters or Setting in Hyperterminal
Check parameter N112 to N113
You can use these paramters below these work nice for me.you could lower the baudrate to 300 instead of 2400 as a test. But 2400 works for me. Use a short cable if possible.

N112=1 (Means language set to ISO)
N113= 1
N114=30
N115=1 ( Means 2=stopbit)
N116= 2400 (Baudrate in)
N117= 2400 (Baudrate out)

do you have these settings? the you could set up you hyperterminal As I described on the web page.

Remember to set Parity= Equal

open Hyper therminal choose "properties" and "settings"
control that:
"Terminal keys" are checked
"Ctrl+H" are checked
emulation = ANSIW
Telnet terminal ID= VT100
Backscroll buffer lines 500
Input Translation Shift-JIS
Check send line ends with line feeds
Check Echo typer characters locally
Line delay 0
Character delay 0
check wrap lines that exceeds terminal width

[parveenk78]

thax for giving me details i will try ..and if you have a post processor for VISI CAM then please write me soon ..
thax
take care

[smoregrava]

I don't hav any experienses with VISI CAM

[parveenk78]

Dear Sir,
thax for reply my message. i talked to my dealer about this post proccessor i have a a complete seat of VISI CAD CAM and MOULD DESIGN. so he can help me about this post. but he also don't have any exp. with maho . so he need a complete program of this controller so that he cam study the nc file and can made the post . so i m requesting you please send me any complete program to me which should have milling drilling operation and have circular interpolation also i mean a complete file it will be help full for me .
i m relly thank full for this discussion with you .
thank u so much in advance
Take care
Parveen

[smoregrava]

Yes I send you a program to morrow. you find some examples on my site. Drilling examples.

I never do drilling and milling in the same program because I don't have toolchanger so. Drilling is one program a milling another program.

He should check the site to find all the M and G codes He will need that.

And maybe the moust important thing. Y and Z axis has to be exchanged and X axis has the opposite direction.

would you share your post with us when it's done? I would like to have it on my web page.

[smoregrava]

Here is a engraving of ligthning mcqueen. should have moust of what you need togehter with the web page.

http://smoregrava.net/Maho/mahomh500.htm