Worries with post pro mazak Mill turn QTM / Haas ST

[usivar83]

Good morning all,

I encounter a problem when using the Post Pro below.

https://cam.autodesk.com/hsmposts?p=mazak_quickturn&_ga=2.43605606.2137178648.1581796854-1513531034....

I would like to make an adaptive blank, in order to machine the following parts:

Only, when I seek to post process the tool path, I would like to use only the C axis and avoid the Y movements. My solution was to use the Pro QTM post.

But when I machine my parts, the machine goes out of stroke.
Indeed, looking at the G code, the C axis does not perform a full rotation and the machine is therefore forced to descend below the X axis. Voici le G code a gauche celui du mazak, a droite le Haas : 

I hope you will be able to help me, when I post one with a Post Pro Haas, I do not encounter this problem.

Sorry for My English i'am french ! 

Thank you in advance and wish you a nice day.

[Anonymous]

You need polar coordinate activated to run that code, that's why you don't have a problem with output from Haas post.

In Fanuc and Haas control G12.1 (G112) starts polar coordinate and G13.1 (G113) cancels it. I don't know what equivalent is for that function on Mazak control but your machine manual should provide that information.

[usivar83]

Hello Vickosta,

A big thank you for your reply !

Only unlike the Post Pro Haas, "Use Polare coordinate" is not offered on the Post Pro Mazak in the link above.
In any case, there is no easy access.

I tried to add this code (G122 replace G112 on Hass / Fanuc) directly in the program but without success, the machine still drops in X-50 is below its capacity. Maybe it should be added to the post pro before editing the program?

In addition, I notice that on the Haas edition which seems to work, this code G112 does not appear.
There was also no activity in configurable properties.

Thank you again for your response!
I really hope I can fix this problem 🙂

Have a good day

[Anonymous]

---

@usivar83 wrote:

Hello Vickosta,

A big thank you for your reply !

Only unlike the Post Pro Haas, "Use Polare coordinate" is not offered on the Post Pro Mazak in the link above.
In any case, there is no easy access.

I tried to add this code (G122 replace G112 on Hass / Fanuc) directly in the program but without success, the machine still drops in X-50 is below its capacity. Maybe it should be added to the post pro before editing the program?

In addition, I notice that on the Haas edition which seems to work, this code G112 does not appear.
There was also no activity in configurable properties.

Thank you again for your response!
I really hope I can fix this problem 🙂

Have a good day

---

G12.1 is equivalent of G112 which I see in your first post screenshot, G113 is equivalent of G13.1

I don't run Mazaks so I don't know how this is handled but I assume there is a code that serves same purpose.

In polar coordinate tool never crosses part center line, built in function of polar coordinate is to rotate C axis instead so that tool always works on positive side of X axis. 

[usivar83]

Thanks again for your quick responses!

Here is what I find in my mazak book:

- G12.1 polar interpolation
- G13.1 Cancellation of polar interpolation

- G122 Mode of introduction of Polar coordinates
- G123 Cancellation of the polar coordinate input mode

I'm sorry, I'm a beginner in ISO, I always work in convertational!

Can you confirm the possible solution to add a code after having post process? If yes which one and at what level of the program?

The post pro being processed, can I expect a final version that will work without modification?

Thank you very much !

[Anonymous]

So it appears that your Hass post is just what you need, produce tool path as you normally do, post using Haas post processor then edit any codes for initial functions, such as turning on C axis and performing zero reference, turn rotary tool on, get in position then start polar coordinate by entering  G12.1 on single line.

After completing work, retract tool in Z axis, cancel polar coordinate by G13.1, stop rotary spindle and unclamp C axis, retract turret to safe position.

That's the process outline, you have to look up your book for proper M codes to manage C axis and rotary tool, I don't have that information.

[usivar83]

I did a lot of testing but these changes are not at my level 😞

Do you think that I can hope for an update of the post pro so that it is operational easily without modification?

Thank you again for the time spent. It seems to me that Bob Shultz is working on this pro post?

Thank you !

[Anonymous]

What I was saying is, use your text editor to modify M codes that your machine requires to perform those functions.

You can produce tool paths in half dozen post processors then adopt it to your machine by changing few codes that drive your machine's C axis and rotary tools.

For instance, I have Yama which uses M19 to engage C axis and Hyndai uses M43, these codes are specific to machine tool brand so you just look up your book for that info and edit G-code after posting with Haas or other post. 

HSM library does not have post for Mazak so you have to find way around it or somehow get the right post.

[usivar83]

Hello,
Thank you for your answers, the solution in my case was to manually add NC Command!

UsePolarecoordinate and UseZXCMode

Placed before each milling unit, everything goes nickel!

Thanks again for your answers!