Emco Maier Compact 6p 120p lathe post processor including results

[DaneelSE]

Welcome to my second post processor project.

The Machine:

Emco Maier Compact 6p sometimes called Compact 6 CNC P or Compact 120p

The controller is an old TM01, so beware if your machine has a more modern TM02

My lathe's controller software revision is:

AC03.02/DC03.05

Some basic facts about the machine:

Working area

• Swing over bed 180mm
• Swing over cross slide 75mm
• Max length between centers 180mm
• Max diameter of workpiece 90mm

Main spindle

• Through hole 21mm
• Speed Range 80 - 4000 rpm
• Manual chuck 80 / 85mm
• Pneumatic power Chuck (without through hole)
• Pneumatically operated tail stock

Automatic tool turret

• 4 external tool holders (12mm shank)
• 4 internal tool holders (16mm bore)

Main drive

• 2 kW DC motor

Feed motors

• Feed 1-1200 mm/min
• Resolution 0.001 mm
• Feed Power 2000 N
• Rapid traverse 1200 mm/min

As the new forum don't permit editing of posts (I think) the updates will be below newer posts. A useful status update should have a summary of:

What's been tested, the result, suggestions or questions on how to proceed and maybe a attached file of the success, disaster and or a new post processor file.

At the moment the postprocessor is in early development and can't be used.

What is working (afaik):

• Program header
• Formatting of code (NXXXX<space><space>G-code)
• Linear interpolations

What is missing or not working:

• Tool change, Need some type sequence here, maybe M00 then move to safe position, make tool change and force new G00 to entry position
• Ending of program move to safe position, reset offsets and turn off spindle
• Drilling cycle
• Threading cycle
• More cycles?
• Update the description in the post

[DaneelSE]

---

@PantechniconDesign wrote:

Hi Daneel,

Thanks for making the Emco post, I'm using a 120P with a T1 control.

---

No problem, I am posting this to get help and feedback. Now I'm getting feedback, I like it!

---

@PantechniconDesign wrote:

Can you tell me how you are creating your drilling cycles?  I'm getting some odd results in the post.

I would expect to get something like this

N46 T0808
N48 G97 S1000 M3
N50 G95
N52 G0 X0 Z46.
N54 G1 Z16.15 F300
N56 G0 Z46.
N58 X30. Z40.

But instead I'm getting this:

N0270 T0808
N0280 G54
N0290 G94
N0300 G97 S3000 M03
N0310 G00 X0. Z50.24
N0320 G00 Z40.08
N0330 Z50.24
N0340 Z40.08
N0350 G87 Z18.897 F1000.
N0360 G00 X0. Z50.24

In the simulation the drill toolpath is in the correct position, but in the post it is too far out in Z.

Any ideas?

Cheers,

Jacob

---

---

I can see why you are not happy. I tried to replicate what you are doing. I think it is a simple Drilling - rapid out cycle, right?

The toolpath from the cycle is looking like this:

 

 What is posted out from the Emco we created and the standard Fanu Turning post is:

---

---

I agree that when you look at G-code both from the Emco and the standard Fanuc turning post processor it is hard to understand where all the movements are coming from when you compare it to the toolpath.

If you compare the output of the standard Fanuc to the Emco, they do look very similar. So in this case I hope that it is one of your offsets that is too far away? If you move the clearance plane to the same as retract plane you should be getting less Z movement. So try setting the clearance Height offset to 0, and test to post out again.

 

As you can see above the jumping back and forth is now also gone.

I hope this helps? 

[PantechniconDesign]

This works. Great, thanks!

[Paulius-UP17]

Nice job!

Thanks for putting effort to write and share post processor for Emco.

There is updated version.

It fixes Arc interpolation (G02-G03) problem.

[hahn_rossman]

Here is a version that works on my Emcoturn 220p. I tried to add a lot of comments to show what changes we added. 

Hahn Rossman

[hahn_rossman]

Latest version for the 220p! Includes the fixes for strange behaviors involving G02/03. Thanks again to everybody involved.

Hahn Rossman

[Anonymous]

Hello!

I am tinkering with a Emco compact 5 cnc and would like to be able to use Fusion 360 to generate g-code for the lathe.

This is a totally new area for me and postprocessors is something I dont quite understand. Is there a short answer to how to make or modifying a post processor to work with the emco 5?

[robin.impey]

Mangep, I have recently been given a working Emco Compact 5 CNC and hoped to use Fusion 360 to generate code but found there is no post processor. Have you made any progress?

Robin

[hahn_rossman]

@Anonymous @DaneelSE 

The postprocessor I attached further up in this discussion works great. There are some differences between the TM01 and TM02 control that are commented in the code. 

@nyccnc has a great youtube video or two about modifying post processors for fusion/HSM. 

Good Luck!

Hahn Rossman

[Anonymous]

Hallo Sir, zuerst a, war Sie ein glücklicher neuer Jear!

Ich habe den Download von Ihrem Programm Emco-Compact6p_vert.cps. Es funktioniert sehr gut, und ich will Ihnen ein großes Kompliment für aussprechen.

Ich brauche yor Hilfe in Postprozessor Emco wird 120!

Pleas schauen sich das Bild an. Ich hoffe, Sie werden mir helfen!

Die linke Seite des Bildes ist die Ausgabe von meinem Programm, aber ich brauche es wie die rechte Seite des Bildes.

Ist es möglich, das Programm so zu ändern, wie ich es brauche?

Danke Stefan

[DaneelSE]

It seems Stefan ran in to the old G02/G03 bug, thanks for fixing it Hahn!
Attached to this message is basically the last version Hahn Ross worked on.
Stefan had another request in a private message, it was to add the extra Modal offsets for
G57 through G59 to the code.

I can't really find any other way but to add it as a extra property during the post dialog.
So it is in there now and disabled by default.

I think the idea from Emco was to have a fixture offset (like vice or chuck) and then a work offset from the bnase of the fixture. So G54 and G55 is in one modal group and G57 to G59 is in another. To use the optional G57 to G59 enter the offset and turn it on in post processor parameters as shown in the picture.

[DaneelSE]

Some more formatting changes

I moved the output of the cad data to after the program start.

I added option to disble parts or all of the comments as seem to generate issues for some. 

I also added code to prevent work offsets above 2.

Let me know if there is anything else we need to work on.

[EmcoAlex]

Hi! I got a Emco Turn 120 with tm02.

without pneumatic!

do i need to edit this pp or should it work?

this is the only one pp for emco tm01/tm02 right?

thanks

[mayr_t]

I've edited the Version 24 of this postprocessor. I’m using it with an Emcoturn 120 with a TM02 control.

I implemented taping and taping with chip breaking.

I also changed the thread turning cycle. Now it uses the G33 instead of the G85.

The benefit is that this cycle works the same on the TM01 as on the TM02.

I deleted the drilling and boring cycles, so they are expended and then done by G01 and G00 commands, which I think works better, but also needs a bit more program storage.

For me it works perfectly, but there’s no guarantee that it works on other machines/controls.

[DaneelSE]

---

@mayr_t wrote:

I also changed the thread turning cycle. Now it uses the G33 instead of the G85.

The benefit is that this cycle works the same on the TM01 as on the TM02.

Great work @mayr_t !

I have a turning project coming up so I'll give it a try when spring heats up my workshop.

Did you validate any turning options? left/right hand threads. Left and right hand tooling?

---

@mayr_t wrote:

I deleted the drilling and boring cycles, so they are expended and then done by G01 and G00 commands, which I think works better, but also needs a bit more program storage.

---

Sounds good, a working post processor with all options using a bit more rows is a good post processor!

Is there anything else you have found funny or not working when using it?

[tom_bresenhuber]

Hello guys,

I just bought an Emco 220p and was wondering if anyone could recommend a USB to serial adapter + cable?

Which program do you use for file transfer?

Thank you tom

[tom_bresenhuber]

So, I have some form of communication working. If I send data from the EMCO to the PC, it works perfectly, but the other way around, it doesn’t.

I am transferring data using Tera Term with the following settings: 300 baud, 7-bit, even parity, 1 stop bit.

On the EMCO, the settings are:

• O.00 = 4 (I also tried 0 and 1)
• O.01 = 121

I have already tried various combinations, but either I get ERROR 600 or nothing happens, and the number 053248 is displayed on the screen.

What settings are you using? And what cable setup do you have? (I have only three pins connected: 2-3, 3-2, 5-7).

Please HELP!

[PantechniconDesign]

We no longer have this machine, but this may help. We were using an Rs232 adaptor and crossover cable, the company that made what we were using is no longer in business.

 

[DaneelSE]

This is the cable I have been using for many years, I hope this helps.

Emco - PC
DB25M - DB9F
RXD 2 - 3 TXD
TXD 3 - 2 RXD
CTS 4 - 7 RTS
RTS 5 - 8 CTS
GND 7 - 5 GND

PC - Emco
DB9F - DB25M
RXD 2 - 3 TXD
TXD 3 - 2 RXD
GND 5 - 7 GND
RTS 7 - 4 CTS
CTS 8 - 5 RTS

[tom_bresenhuber]

Thank you for the response, i checked the cable and it should be the right one.

What program are you using for transferring the files? TeraTerm, Hyperterminal,...?

What are your settings?

[EmcoAlex]

you need a cable with profilic chipset

 StarTech.com 1 Port USB auf Seriell RS232 Adapter - Prolific PL-2303 - USB auf DB9 Seriell Adapter Kabel - RS232 Seriell Konverter (ICUSB232V2) https://amzn.eu/d/de4M9bB

i use this. original this blue from startech.com bought at amazon.

you need more then tx rx crossed. you need the handshake. buy this cable and then i can help you to setup teraterm and your machine.

ok?

i forget!!!

you need male db25 and female db9 connector.

you must solder a converter.
i can help you for this. easy job.