Hurco Max mill control and MC

[Paul_RagotCADCAM]

Hi,

 

Anybody using MC to program a Hurco Max mill control?

What do you use for post? A g-code like the mphurco on the CD or conversationnal?

 

What is the best way to program it?

Do you need to buy the ISNC (Industry Standard G code package)?

 

What is the best way to run long 3D programs on it?

- zap them in via the Ethernet option or drip feed?

Is drip feed standard?

 

Any options recommended for doing 3D work?

 

Paul

[specprogrammer]

Paul, we have two HURCO ultimax VMC's. We do a lot of 3-D work we send the code via ethernet. The mphurco post is what we use, and select industry standard from the options on the touch screen. If these Hurcos are similar that should work for you.

[Paul_RagotCADCAM]

Thanks.

 

I called up the tech guy at the dealership and he was pretty helpful:

- use the mphurco, works well with HNC (Hurco NC) which is standard and good for 3D work

- ISNC is optional. Allows to run Fanuc and macros.

- drip feed is standard but with 55Mb RAM, not really useful unless you get into really big files

You can always start the program while it is loading via RS-232.

- Ethernet is nice to have but requires FTP software on PC

 

Paul

[Midwest]

quote:

---

Ethernet is nice to have but requires FTP software on PC

---

You can download the software free from the internet. I'm not at work right now, I'll try and get the web site when I get back to work if you would like, let me know.

 

 

[pip]

We dropped our ethernet connection in favour of the Fanuc interpreter.. Watch your code very carefully with the Fanuc option. In MC the code veryfied to perfection, but on the machine the job was scrapped. We have purchased a post for our Hurco VMX42 and when the Hurco encounters a line smaller than the radius of the tool, it does not alarm out. It tries to reposition itself at a tangential start point to the line, and hey presto. One more scrapped part..

[Midwest]

Here is the FTP software we use.

 

click here

 

 

HTH

[specprogrammer]

pip, I have had the same problem before. It seems to always happen when using cutter comp. Its the lead in/out that it has problems with. I go in and change those values and repost. See if that will work for you.

[Racer X]

I just purchased a Hurco VM1 with the Max control. Also, I bought the ISNC. I received two posts from my dealer. One is the standard mphurco post, the other is called hurcoisnc. The isnc one is the one I have used thus far. Still trying to tweak it a little although it is very close. If you want the hurcoisnc one I would be more than happy to share with you. Let me know.

 

Cheers

[Midwest]

Moto GP,

 

We have a Hurco VMX42 with ISNC I have never gotten it work safely because of Z axis wild radiuses. I didn't know they had a hurcoisnc out there. If you would E-mail me it I would really appreciate it.

 

[pip]

Motogp I would be very interested in looking at your post. Unfortunetly I cannot share ours as it is protected by our supplier.. Which is an absolute bummer, as I have become quite good at post editting, and have adjusted severall post, including 5 axis posts. As ours still needs a couple of edits, I have to wait until our suppliers is able to visit us..

P.S this is not a complaint about our supplier, our IT department is very slow at getting things done..

[Racer X]

Pip,

 

Send me your email address and I will fire the post off to you.

[specprogrammer]

Midwest, We had that problem also. I believe that the "Z axis wild radiuses" problem is solved by changing the swg 18 variable to a 1.

[Midwest]

Moto GP,

 

I sent my E-mail address to you

 

Thanks

 

[Midwest]

Specprogrammer,

 

I'll try messing around with the swg 18 variable.

 

Thanks

 

We also have an older Hurco. We had the same problem with it several years ago. It's hard to remember the changes I made back then to solve the Z axis rad problem. I might try comparing the hurco original post to my current one. I think it was something about writing the code at every quadrant.

 

We also have a Haas, that is the post I originally tried with the ISNC side. I was hoping that post would work in both machines. That way someone could set-up either machines and use the same post, but it didn't work. So I dicided to stay with the hurco post and use the Hurco nc side. We were really busy and didn't have time to play with it.

 

Hope that all made sense

 

[lynnz]

Here is a fix mentioned 3 yrs ago for Hurco posts. It stopped the 'wild arcs" problem for us.

 

"If you are using the Mphur.pst, search for the note on 'swg18'. The hurco and boss controls reverse the G18 plane definition from what the rest of the industry uses. Set 'swg18' to 1 from 0."

 

Good luck.

lynnz

[Midwest]

Moto,

 

Been trying the hurcoisnc with some old jobs to test for problems and I get this.

 

 

I went back to the basicnc side and posted with the one I have been using and it ran fine.

 

 

The bright spot is the flash when I took the picture from the Hurco screen.

 

Maybe I'll just leave the ISNC side alone and stick with what I have, so far it has worked every time.

 

Becareful with your post

[Karl Oram]

Hi Guys,

I have a customer using this control and was also getting the wild arc moves using mphurco. I took mpmaster turned on the break arcs to quadrents amd with a few little changes it seems to be working great.

 

Regards Karl

[Chip-pan]

I've seen it where the screen on the hurco says one thing and the tool movement does another, and vise versa !!!

 

Chip Pan

[specprogrammer]

Midwest, on your pocket toolpath, go to the "Roughing/Finishing parameters" tab and check "lead in/out" and assigning parameters to it and you will solve the wierd XY loop problem.

SWG 18 will solve the loops in Z and lead in/out will solve XY loops