[neurosis]

We are looking in to a new Horizontal machine and have been looking very closely at a HCN-4000 II. I dont have any experience with Mazak machines at all so I dont know what to expect out of this control.

My questions are about the processing speed. We do quite a bit of high speed machining and a fair amount of 3D contouring. We use mastercam as our programming system. It was recommended to me to purchase at minimum, the fine spline interpolation for this machine and even suggested that we get the 3D high speed software package.

Now we do "NOT" make molds. On other machines that we have looked at, they said that the 3d was only required for the smooth surface requirements that come with mold making.

Anyone that runs one of the new Mazak controls that could offer advise, suggestions, or any insight on the processing speed of these controls would be appreciated. I read that the control only has a 3 line look ahead which seems very low compared to any other machine that we have compared it to. Most has 30 - 80. One even had 300.

Thanks.

[MrMazak]

I have four HCN400II's and the standard high speed machining package using G61.1 is all you need for most high speed and 3D contouring needs. I don't see how the fine spline interpolation would help with your application but you could add it at any time for $3260.00. The MAZACC-3D package for mold making is $3370.00 but is only for extreme speeds like graphite machining and could be added in the field also. As far as the control speed, I have many M640 controls and they don't even come close to a Matrix in high speed contouring.

[neurosis]

one more question for you if you could.

I had someone also tell me to make sure that you could program for tool breakage detection in the EIA side of the control. This is very important to me that this works. The person that suggested that I look in to this, said that they have never been able to get a straight answer on the subject. This is a must for us.

I should post this as a separate topic. I may here in the future. Can you give me any insight as how the tool breakage detection works in the EIA side of the control? Is it possible? Easy?

[arie2003]

hi neurosis,
it's possible to use tool breakage detection in EIA, but it's quite difficult because you must have some macro program to make it run.
The easier way is use Mazatrol subprogram for tool breakage detection (TBR) and call it in EIA main program. You only need to command M35 in Mazatrol to run TBR.
I use this method in several machine with Matrix controller.

[neurosis]

hi neurosis,
it's possible to use tool breakage detection in EIA, but it's quite difficult because you must have some macro program to make it run.
The easier way is use Mazatrol subprogram for tool breakage detection (TBR) and call it in EIA main program. You only need to command M35 in Mazatrol to run TBR.
I use this method in several machine with Matrix controller.

Do you do most of your programming using Mazatrol? Or do you mix EIA and Mazatrol? Is it easy to create a Mazatrol program that calls to EIA programs?

We do 100% of our programming with Mastercam. I dont think that we will be programming much of anything using the Mazatrol so it is very important to us that we are able to get the TBD working using EIA. I plan on learning the Mazatrol side of the controller but I do not want to have to rely on it for my programming needs if possible.

Another thing that is important to is will be fixture offset adjusting using a touch probe. We would like to be able to dial in parts using the touch probe and have it automatically adjust our fixture offsets accordingly. So far I have not got a comprehensive answer on if, how, or even what it takes to get this working. Every time I ask about it, they just nod their head that it works but dont look certain of themselves when I ask. They also have not explained how to make it work which worries me.

Has anyone had any experience with that? (fixture offset adjusting using spindle probe)

[psychomill]

it's possible to use tool breakage detection in EIA, but it's quite difficult because you must have some macro program to make it run.

No no no no no...
It is very EASY to run. When you buy the EIA tool breakage option, Mazak supplies the macros and it's already loaded on the control for the U.S. machines. I don't know about Asia though.

As for the High Speed machining. I'm constantly running at high speeds/feeds. G61.1 will take care of 99% (if not 100%) of what most shops do. Mazak needs to update their books about Look-Ahead because none of them have been right for about 10 years plus. I think somebody keeps copy/paste the crap from older text. Also, the verbiage isn't exactly correct either. Bottom line, stick with the G61.1 for now if you like. Both Spline interpolation and 3D contour (G5) can be added later. It's only software stuff.

Now, Spline interpolation is a much faster program than the standard linear 3D. This has to do with code processing and this is for ANY machine control. Mazak, FANUC... whatever. It doesn't matter. There are certain restrictions and rules though to run this and be able to comp which is why many people do not use this option on any given machine/control. Plus, the CAM system used needs to be able to output spline control points for the machine to run (which MasterCam can). Stick with G61.1 and go from there....

Mazatrol and EIA can go back forth in a program. I don't program Mazatrol on mills for 100s of reasons but I might use it for a quick fix or fixturing. Don't get me wrong... there are many shops that use Mazatrol exclusively on mills and even run a good deal of 3D with it. I prefer EIA for many toolpath control reasons though. But if you wanted to, you can subprogram back and forth all you want.

As for probing..... Mazatrol is already set up for probing you have at least that. You only need to buy the probe from Mazak. You can buy it yourself but then you have to set it up, configure, etc, etc. Easier to have Mazak do it when they install the machine. For EIA probing though... Make sure you order the Renishaw Inspection Plus option from Mazak. This will give you the probe and all of the macros for probing. Mazak or Renishaw will install and configure the whole thing during machine install. It does work and it works very well. I've been running probes on Mazaks for more years than I can count. The option also includes probe training by Renishaw on site. While you're at it, you may want to take a look at tool setter options (laser setter and other EIA options for this stuff).

[Integrexman]

For EIA probing though... Make sure you order the Renishaw Inspection Plus option from Mazak.

I just bought the Renishaw Inspection Plus Macros for our Mazak Vortex Mill and it was about $250 less to get them from Renishaw ($1076) than Mazak. I would definitely get a Probe and the macros. You will never need an edge finder or indicator again. Plus you can also make programs to inspect 3D points (XYZ) with macro 9821 like a CMM. I just started doing this and it works really well. If your CAM system can output XYZIJK point data for a CMM I have made a program that takes the point data and creates a G-code program using the 9821 macro to inspect parts in the machine. The Instruction Plus software has a macro that will create an inspection report.

[Integrexman]

Here is the program I use to generate probing cycles for my machine.

http://cncwrite.com/cmm.php

[yepingapple]

For Mazak option in Matrix system, I can edit (increase or decrease the option) freely !

If someone need option, can send the machines information include: S/N, opt file, option item to my E_mail : [email protected], I will answer for you next day.


Can someone tell me how to read the tool length of tool breakage measuement in Magzine side of HCN-6000II ?

Have some D address ? or Variable ?

Thank you !

[XRACERJB]

we have a brand new nexus 510c with the renishaw probe upgrade running in EIA and all we did for tool breakage detection was this G0G91G28Z0;
M350; still new to the mazak think but reading the manual will get you very little. I've learned more reading on here in 1 HR. than 2 days of the manuals. Thanks CNCZONE

[yepingapple]

Dear ,

Thanks a lot !

Actually, M350 is most important !

It is a macro command !
It include so much info, and maybe very difficult !

Can you share us all detail info of M350 ?

Thanks !