Output b-axis degree on a Mazak Horizontal HCN-5000

[Dreas]

Hello,

 

i have a problem with our new MAZAK HCN-5000.

It's a Horizontal machine with a index table of 0,001 degrees.

If you like the b-axis to go for example 45 degrees you have to program b45000.

On our older MAZAK PFH-4800 we have a index table of 1 degrees.Here you have to program b45.

The PFH-4800 has the controler 640M and the HCN-5000 the Matrix.

 

Someone of the MAZAK users can tell me a parameter where i can change the HCN-5000 to program also with b45 ?

Because i don't want to change all my programs and can program both machines with one post on Mastercam.

 

If there is no way to change a parameter on the machine,

where can i edit the mpmaster to ouput the b-axis with that format of 1000 ?

 

Thanks

Dreas

[huskermcdoogle]

Hello,

 

i have a problem with our new MAZAK HCN-5000.

It's a Horizontal machine with a index table of 0,001 degrees.

If you like the b-axis to go for example 45 degrees you have to program b45000.

On our older MAZAK PFH-4800 we have a index table of 1 degrees.Here you have to program b45.

The PFH-4800 has the controler 640M and the HCN-5000 the Matrix.

 

Someone of the MAZAK users can tell me a parameter where i can change the HCN-5000 to program also with b45 ?

Because i don't want to change all my programs and can program both machines with one post on Mastercam.

 

If there is no way to change a parameter on the machine,

where can i edit the mpmaster to ouput the b-axis with that format of 1000 ?

 

Thanks

Dreas

 

 

As Far as I know you can't change it on the machine. We had the same issue the issue you have is you have the NC positioner, not the nc rotary table. I just changed my post and let it ride. To change the post look at the link to the post I started on practical machinist two years ago. Its just a format statement. Pretty simple fix just don't remember the details off the top of my head.

 

Post Format Issue - Practical Machinist

 

 

Good Luck

 

Husker

[Dreas]

Thank you Husker,

 

so i know i have to edit the post, because there is no way to change it on the controller.

I will try output the b-axis as a parameter like #132.

Than i will set a parameter in the controller on the PFH-4800 #131 to 1.

Than i will set a parameter in the controller on the HCN-5000 #131 to 1000.

So everytime Mastercam is output a rotation ,like for example, 45 degrees

the nc code is

 

G00 G17 G21 G40 G80 G90

G91 G28 Z0.

T13 T14 M06

G91 G28 Z0.

G28 X0. Y0.

#130=45

#132=#130*#131

G90 G54

B#132

 

With that i can program both machines with only one post.

[huskermcdoogle]

Thank you Husker,

 

so i know i have to edit the post, because there is no way to change it on the controller.

I will try output the b-axis as a parameter like #132.

Than i will set a parameter in the controller on the PFH-4800 #131 to 1.

Than i will set a parameter in the controller on the HCN-5000 #131 to 1000.

So everytime Mastercam is output a rotation ,like for example, 45 degrees

the nc code is

 

G00 G17 G21 G40 G80 G90

G91 G28 Z0.

T13 T14 M06

G91 G28 Z0.

G28 X0. Y0.

#130=45

#132=#130*#131

G90 G54

B#132

 

With that i can program both machines with only one post.

 

 

What will the PFH do if you command 180000 with no decimal place? Is it a full fourth on the PFH? If it goes to the right place why not just let it ride and use the format for the HCN?

 

 

Husker

[Dreas]

The PFH is not a full fourth.It's only a 1 degree indexer.

I tried input 180000 with no decimal place, but all i get is an alarm.

I think the machine wants to go than 180000 degrees.

We program the b-axis on the PFH always without decimal place.

Maybe i have to change parameter F91 Bit5.Have a look tommorow on the machine.

But if i change the paramter it's dangerous when somebody ran an old program on the machine.

The machine will then index only 0.18 that's like nothing !

I've also tried change parameter F91 on the HCN with no luck.