[pontiacg5]

Is there a way to make a post processor file for both T and M plus mazak controllers? For some reason I was thinking that mazak used Faunc controllers but I don't know if that is right or not
Is there any particular place I should start? I've got a bunch of machines so I don't know that listing all of them would help, but I can if I need to.
A little guide or something similar would be perfect.
Thanks!

[Brakeman Bob]

I may be wrong (it has been many years since I laid hands on a Mazak) but isn't the T Plus a turning (or Mill-Turn) control and the M Plus a milling control? I presume you would be programming in ISO and not Mazak's conversational language and therefore the would be different G & M codes required for turning & milling.

You can structure a SolidCAM post for both controls because that is how the Mill-Turn posts are constructed but it means that every part you program in SolidCAM would start life as a Mill-Turn part.

In a scenario with many different machines (even ones from the same builder) I find it pays to have separate posts for each machine / control. For example, I program for 3 Mori Seiki 's. a SH400 and two MH40's with the SH and one of the MH's having Fanuc 16MA whilst the older MH has Fanuc 0M so I have two different posts, one for the 16MA and one for the 0M.

If you have different machines that share the same control for example a QT10, a SL30 and an Integrex all with T+ then it is possible to merely have 3 different MAC files all referencing the same GPP file and local differences handled in MAC variables.

Finally, some Mazaks did use Fanuc and the ISO side of Mazatrol is very, very similar to Fanuc but be aware that it isn't identical. I once saw a spindle on a HV800 destroyed because the period of dwell in a G04 call isn't designated by a Xn word, but by a Pn - we were tapping with a right-angle head at the time and the "G04 X20." call moved the head about 300mm through the job. Big bang! Disintegrated RA head! No spindle! Very glad it wasn't my code......

[pontiacg5]

I wouldn't mind making a processor for each one, but I would like to know where to start.

For example, I have a SQT-10M that has the T Plus controller. If I wanted to make a Post for that machine what information would I need and how would I go about making that post.

I guess I'll start with the easier lathes and work my way up to the nexus

[Brakeman Bob]

Start with a generic FANUC turning post.

I would suggest that you create a test part in SolidWorks and then program it in SolidCAM. This part would have all the features that you need specific types of code for eg rough turning, finish turning, drilling, boring, chamfers, rads - everything that you code for at the moment. Post it out with a FANUC post and compare the code to what you think it should be - even go as far as programming your test part by your existing method and proving out on the machine if you have to. In fact, this latter is a good idea as it will give a reference of what your posted code should look like.

Then make copies of the FANUC MAC and GPP files calling them "MAZAK_turn" (the underscore is important - there are parts of SolidCAM that can't cope well with spaces in text). Alter these copies after studying the GPP help and making use of the numerous post-tweaking threads on this forum. Keep editing, posting and comparing until the post gives you the same as your reference program.

A word of caution. Start off by posting code without using turning cycles such as G71 etc. These use something in GPP called "PROCS" (short for procedures) and getting procs right can drive you around the bend to begin with.

As for machine information, well you will need the Mazatrol T-Plus EIA-ISO manual that's for sure as this will give you the syntax of the code; as I said in my previous post, Mazatrol is very similar to FANUC but not identical. Other info you will need is pretty self explanatory in the MAC file, stuff like maximum rpm, axis limits etc.

have fun

Bob

[pontiacg5]

Start with a generic FANUC turning post.

I would suggest that you create a test part in SolidWorks and then program it in SolidCAM. This part would have all the features that you need specific types of code for eg rough turning, finish turning, drilling, boring, chamfers, rads - everything that you code for at the moment. Post it out with a FANUC post and compare the code to what you think it should be - even go as far as programming your test part by your existing method and proving out on the machine if you have to. In fact, this latter is a good idea as it will give a reference of what your posted code should look like.

Then make copies of the FANUC MAC and GPP files calling them "MAZAK_turn" (the underscore is important - there are parts of SolidCAM that can't cope well with spaces in text). Alter these copies after studying the GPP help and making use of the numerous post-tweaking threads on this forum. Keep editing, posting and comparing until the post gives you the same as your reference program.

A word of caution. Start off by posting code without using turning cycles such as G71 etc. These use something in GPP called "PROCS" (short for procedures) and getting procs right can drive you around the bend to begin with.

As for machine information, well you will need the Mazatrol T-Plus EIA-ISO manual that's for sure as this will give you the syntax of the code; as I said in my previous post, Mazatrol is very similar to FANUC but not identical. Other info you will need is pretty self explanatory in the MAC file, stuff like maximum rpm, axis limits etc.

have fun

Bob

How would I compare the codes? I don't have any G-code to reference to, only the mazatrol code.

[Brakeman Bob]

Then I presume you have only ever programmed in Mazatrol conversational. If this so you have two choices, either learn to program your machines in G code or give up on trying to use SolidCAM for programming your Mazaks. Mazatrol conversational is (or was - it may have changed) a sealed proprietary format and as far as I know only Griffo Brothers offer a product for offline programming Mazaks in conversational.

It used to be that you couldn't even read Mazatrol on a PC as it is in binary format.

[pontiacg5]

I've only used mazatrol so far, but I would be willing to learn G-code if it is necessary.

I'm confused though, is G-code a standard code or do all machines run it different? What is the purpose of a post processor if G-code is a standard code?

G-code looks to be a little more difficult than mazatrol, which is why I wanted to use solidcam to generate the G-code for me, but it looks like its not going to be that easy!

[Brakeman Bob]

G code is an international standard and is detailed in two very old standards by the Electrical Industries Association and the International Standards Organisation (hence the other name Gcode goes under of "EIA-ISO"). These two standards are very similar (in fact I believe that their only difference lay in the format of punched paper tape and the check digit) but they only cover machine movements such as lines, arcs, rapid feed etc. - stuff like tool changing, assigning offsets and so on was left up to the machine tool manufacturer and they have gone each to their own way. So the positional G code to mill a rectangle will be the same between any machine the code that gets the tool to the right start point, turns the coolant on and takes the tool away at the end is most likely very different. So to get around this problem people wrote post-processors (or "post") that were machine specific. Indeed, you will need a different post for a vertical and a horizontal mill even if they came from the same machine tool builder and have the same control.

If you learn to program in G code you can program almost any machine, not just Mazaks, but you have to know the differencesthat are particular to the machine in question and for that you need to study the G code programming manuals.

You are right about G code being harder to learn than Mazatrol - Mazatrol was designed for that very reason - but it isn't insurmountable. My advice it to get yourself a good G code editor that can backplot code, that is graphically display the code you have written as a toolpath. That way you can check yourself as you go along. Beware though, the most dangerous times in any CNC program are getting the tool to the start of the cut without hitting anything and getting it away. There are lots of resources on the internet for learning to program in G code and the CNCZone is one of the best places to ask questions.