[Rob.S]

Hi all,

This is my first post here so I should start by introducing myself. My name is Rob and I work for a manufacturing company in the UK as a CAM engineer. We have a Mazak J200 which is currently being operated by a machinist using the on board mazatrol control. We are looking into posting from the CAM system we use to the Mazak but I've run into a few issues in my own experience with Mazaks.

Would any of you happen to have a post which works with a mazak controller in EIA format that I could take some of the formatting from? (i.e. looking at opening and closing sectors).

Thanks and Regards

Rob.S

[dak1]

Hi Rob. We have a J300 in operation using strictly EIA generated from Pro/Engineer (which is now called Creo) CAM post processed through Icam. I'm not execatly sure what you're specifically looking for as descrbed by "opening and closing sectors", but would be happy to assist in whatever capacity I could. This is a very finicky control with respect to formatting & we've been through a number of tweaks to the post as a result. I've requested the maojority of those tweaks as post maintenance is no longer my responsibility. Give me more detail & I'll see if I can help.

Dave

[Rob.S]

Hi Dave thanks for the reply. I've read here and there that the controller doesn't like "%" at the start of a program and won't read it if it's there. I was hoping that someone might be able to help me identify any other characteristics/formatting of a program that are necessary for the j200 to read it. For now the aim is just to write something that the mazak will open file wise.

Thanks and Regards

Rob.S

[dak1]

Rob,

Our original post was developed & purchased externally. The maintenance is now being handled internally so I have access to the history section of the post for the tweaks we've made internally at very least. I don't remember an issue with the original regarding header & trailer info so I may not find anything specific to this. I do recall formatting issues within the core body of the programs that should have some documented information. I'll look through the history comments before I attempt to elaborate. In the mean time, I've randomly attached one of the shortest programs we have for the machine. There appears to be no % at the beginning of the program (as opened in wordpad), but there is at the end, which would support wht you've read. You can see if this program loads ok in your machine. This program may or may not run in your machine dependent on parameters & options. We have the extended (300) fixture offsets & this program utilizes only 1 (P48). It also calls a macro (P9011) for barfeed & uses the multi tip tool option (T001.1) for the cutoff. We use the extended tool offsets as well on all tools (H & D registers) & I believe we execute a macro by G43 to transfer the data from that tool data side into these registers (which you can just supply manually or bypass). There is also a section of polar coordinate interp mode (I don't remember if this was standard or option). Aside from those things, this is a pretty basic program you can try. I had to change the file extension from "eia" to "doc" to get it to upload. Just rename it back to "eia".

Hope this helps & I'll look through our post history comments.
Dave

[Rob.S]

Thanks so much for your help Dave, I'll be looking into the files over the next couple of days. Managed to get one recognised today on the J200 and copied it from usb successfully but it wouldn't animate in the on board graphics. Threw an error 1802 about G12.1 (polar coord interp), which is likely the reason - if it is possible to show the tool paths from the an eia file in the first place?

Thanks again, and regards

Rob

[dak1]

Yes, it is possible. But I don't remember exactly how to get there. I do remember that is is pretty simple to do though. It's just a matter of finding it.

[Rob.S]

Dave, a quick question about the program you've sent me... under N1132 it has a line "G17XC".
Does this activate the x and c axes under polar coordinate interpolation? like the normal plane select of G17 and G18?

Thanks
Rob

[dak1]

Sorry. I've been tied up. Based on memory, Yes. I believe this was in fact one of the tweaks we made but will try to look after lunch.

[dak1]

Rob,

I just looked through the post comments & did not find anything speceific to the G17 code. I found it in a macro, but no comment info. Just going off memory, we put that in to eplicitly specify polar motion be done using the X & C (with Y disabled). If it were a G17YC, I think it would specify Y & C motion with X disabled. Either combination can be used for Z-axis (face) tools. The only case of polar coordinate we use would be the case of G17 using the X & C. We have no example of a G19 type polar scenario (X-axis oriented tool), nor can I dream up an example. This is the best I can do to explain this without studying the manual. I specifically remember this coding being deliberate, possibly as the result of an error, alarm, or a plain machine stoppage without any message or hint as to why (which does happen with this thing). All of our previous mill/turn posts & machines used plain G17/G18/G19 codes without any axis registers added to the code.

Dave

[dak1]

Rob,

I did a quiick search of me email looking for info regarding the G17XC coding, to no avail. I also did not find anything in the post comments about the % sign origianlly mentioned. I was however reminded of a quirk I recently encountered on the machine regarding M200/M202 (MILL/TURN MODE) codes. We hit a M200 code in a program while a G1 was still modally active. The machine issued a 133 alarm (??spindle??) about a dozen lines after this code. After some head scratching the modal G1 was spotted. We changed the post to issue a G0 on the same line as any M200 or M202 code as a global fix.

Unrelated, but within that same program, we were using a C-axis value in the fixture offset (hex stock requiring orientation). The post issues a G53 B?? for tool orientation. Those same lines contained a C?? (ie; G0 C0.0 G53 B0.0 M8). This set the C to machine ref, nullifying the C offset value & throwing feature orientation off. We split the C into a seperate line to corrrect this;

G0 C0.0
G53 B0.0 M8


Did the control load the program OK?