Mazak Nexus 700D-II multiple D offsets for same tool?

[Azoth]

I have a Mazak Nexus 700D-II vmc with a Matrix Nexus Controller.

In my Tool Data page I am missing the "Tool Add" soft key.

On my Integrex I can duplicate the tool using this "Tool Add" soft key so multiple diameter offsets can be used on a single Tool by assigning an ID Code (letter A-Z) and calling up the tool (eg T1.1 - T1.26)

If I remember right, conventionally on Fanuc you can call up unique Diameter and Height offsets in eia programs simply by calling H1 or H11 or H200, but this isn't allowed on this machine either (still using eia programs). It has 2000 offsets available, but only 40 tools and no matter what D offset I put in the g-code, Mazak ignores it and refers to the Tool Data page.

On my Nexus I am able to assign ID Codes and I can call up the specific Tool (eg tool 35 id code G can be called up with T35.7) but I cannot assign multiple letters to the same tool. I must instead stop my program and manually adjust my offset back and forth.

I have checked my parameter book and the parameters that looked related didn't make a difference. And I'm not seeing anything stand out when comparing the Options displayed on my Nexus vs Integrex.

Does anyone know if this function is behind a parameter? or a paywall? or simply not an option on this controller?

 

[noname777]

Mazak Integrex is subdivision of MAZAK, Mills has it own development group. Multitasking has its own. U can see how different electrical and PLC books when it comes to Integrex and Mills.

Integrex is very advanced and flexible machine cause Japanese, sort of realised that it would be incredibly hard to recover "machine crash" mechanically , and the best way to deal with mechanical irregularities and errors would be to create many many parameters and options for people to be able to use upper turret with main and sub spindle.

Fanuc has D and H codes to manage what you need, but than again, Fanuc doesnt make machines, Fanuc creates philosophy of machining. Others just follow it.

 

[CNC Hacker]

Most people accomplish this on those controls by using a combination of the Tool data and Tool Offset page. You can put your main tool length on tool data and do your wear comp adjustments on the tool offset page. Set your parameters like this:

F93 bit 3 = 1
F94 bit 7 = 0

Then at the tool change it will grab the tool length from tool data page, and when it reads a different H or D call up in the program it will add the values from the corresponding offset number you've assigned.

 

[Azoth]

I got a response from a local mazak tech

the Tool Add is a lathe feature, and is not there on mills.

I'll try those parameters but I don't think it's going to work.

F93.3 = 0/1: Tool length of tool data for an EIA/ISO program invalid/valid

F94.7 = 0: effectuates tool offset amount on the TOOL OFFSET display
F94.7 = 1: effectuates tool offset amount for EIA/ISO program on the TOOL DATA display

On my TOOL DATA page, I can set the offset value (eg -.0003) right there on that page or I can give it an offset #0-2000 and it will point to the offsets page, so I think this parameter gets set automatically depending on which text box I fill out on the TOOL DATA page. In both cases, the D word in the program is ignored (it can even be omitted) and it still uses either the D number set on the TOOL DATA page which points to an Offset Value set on the Offsets page, OR it uses the Offset Value set on the TOOL DATA page. I can't tell it T01 G41 D01 on one line then T01 G41 D02 on another.

But I'll try it out just in case.

 

[Nagol]

Yes, sorry to say but tool data add is not a feature on mills until the later model smooth mills. We even have an early 2015 smooth Variaxis that doesn't have it. Our 2020 HCN-6000 can do it so I'm not sure when it started. Sorry this is of no help but just a heads up that they did get around to it eventually.

 

[noname777]

They just accumulated enough complains from customers to pass this issue to the development group to have it implemented.

 

[CNC Hacker]

I got a response from a local mazak tech

I'll try those parameters but I don't think it's going to work.


On my TOOL DATA page, I can set the offset value (eg -.0003) right there on that page or I can give it an offset #0-2000 and it will point to the offsets page, so I think this parameter gets set automatically depending on which text box I fill out on the TOOL DATA page. In both cases, the D word in the program is ignored (it can even be omitted) and it still uses either the D number set on the TOOL DATA page which points to an Offset Value set on the Offsets page, OR it uses the Offset Value set on the TOOL DATA page. I can't tell it T01 G41 D01 on one line then T01 G41 D02 on another.

But I'll try it out just in case.

The offset field on tool data will work like that when both F93.3 and F94.7 are set to 1. If F94.7 is 0 you can change on the fly in the program with D and H calls.

I attached a useful document showing the different combinations.

 

[Azoth]

Okay F94.7 = 0 did tell the machine to read the D word in the program so now I can use one offset for one feature and another offset elswhere. Thank you.

You wouldn't happen to know if there is a way to prevent the machine from cancelling tool height when homing in Z would you? I've been trying to find the parameter for that because it causes crashes. Closest I've found is F94.2 Tool Len. Cancel with G28/G30, but I don't think that's what I want.

Using TPS you can send the tool home but when you go back into the program it picks up where it left off except the Buffer says the next move is Z-.05, but the instant you run that line the Distance Remaining changes to something like Z-12.05 and full send into the part.

 

[CNC Hacker]

I'm not aware of any parameters effecting TPS, I don't use it very often. But I when I have, I always back up like 0.100" first, teach the first TPS point there, then go home and hit it again for a 2nd point. That way the final approach move to the part will be at the programmed feed rate.

 

[Azoth]

It wouldn't be TPS specific. There's no issue with TPS tracing my TPS points back to the part, but it can be deceptive if you send it all the way home in Z because the Tool Length gets Zeroed any time you home in Z as if you hit the reset button. Now that I know that Homing in Z will cancel my Tool Length I'll just not go all the way home in Z with TPS, but I'd rather change the machine behavior to prevent the next guy from crashing like I did.

 

[CNC Hacker]

Sounds like F94 bit 2 set to 1 is what you want then. I checked some machines in the showroom here and they are all set with it to a 1 from the factory.