Configuring and using MC Lathe

[Hugh.Venables]

Hi there you wonderful lot. I need to start using Lathe V8.1.1 as I am even more fed up than usual with the conversational on our Hitachi-Seiki HITEC-TURN 20SII. I'm remembering all too clearly why it spends most of it's time gathering dust. When you manage to get a program going in it it's a really good machine but the conversational........AARRGGHH!!!

 

Anyway, I had a look at MC Lathe and it's set up for inches (horror). I had a look at screen, configure but couldn't figure out what to do. Every time I changed something, closed and opened it had defaulted back to the original settings. I need to configure the dimensions and tools to metric. There doesn't appear to be a metric material library as there is Mill. Can someone please tell me how to do it. Please assume I know NOTHING!

 

Having configured it any words of wisdom on how to become incredibly competent instantly would also be most welcome. I have the V8.1 tutorial book but it is a little tedious.

 

Thanks everyone, have a good wekend, see you Monday.

Hugh Venables.

[Greg Williams]

Hugh,

 

Start by,

 

Screen

Configure

 

Change the pulldown menu on the allocations page to metric and also the pulldown menu on the start exit page to metric. Mastercam will then boot up in metric, As for the tool library I can't help you there as I don't have Lathe

 

[PE @ IHS]

I ran the same lathe with a Yasnac control and it was a damn good machine. I didn't know that they were available in a conversational control.

 

To set your tool library, go to Screen/Configure/Files/

 

in the File Usage window, click on Lathe tool library, then go to the window below and click on the browse button on the right. Find ToolsMM.tl8 and set it as your default.

 

Lathe is pretty easy to learn, even I figured it out. One of the main things to remember is to start with a correct stock definition, including the stock on your face. Set your default ops to always include a bit of lead in and lead out to avoid problems. I would avoid TNR comp and canned cycles unless there is a demand for it on the shop floor (except for threading). The grooving process in Mastercam is really flexible, and even a simple thing like parting off can be done far more efficiently than programming on the control (pecking, semi partoff, break corners, etc.)

 

Peter Eigler

[chris m]

Again I agree with Peter:

 

Avoid tool nose radius compensation like the plague as this can cause weird machine behavior and other issues if not done correctly.

 

Lead in / Lead out is also a must; pick a round # and stick with it [.050" or .100" will make things safer].

 

We don't use Mastercam's corner rounding because it generates a million little moves in every program.

 

Good Luck

[Jim Whipple]

quote:

---

Having configured it any words of wisdom on how to become incredibly competent instantly would also be most welcome. I have the V8.1 tutorial book but it is a little tedious.

---

Uh....Vulcan Mind Meld with James or Jay???

Jim

[EZ3PUTT]

I have spent a number of years programming, set-up and running an HT-20SII. Sure is a nice machine. I agree with the others concerning tool nose radius compensation. I always comp TNR in the computer and never at the control. When using lead in and lead out values direction is an important variable to keep in mind as it can lead to problems if not applied correctly. Our machine has a Yasnac LX3 conversational control that was used before we purchased Mastercam. I don't miss the days we programmed at the control. Our Hitachi is one of the favorite machines in the shop. We make Diesel fuel injectors and this machine will hold tenth's all day long.

[Hugh.Venables]

Thanks guys for your help. Could I just clarify a few things:

 

Greg,

that's the pull down menu at the bottom left of the allocation page and I have to select LATHE8M.CFG (metric), right? And in the pulldown menu at the top centre of the Start/Exit page also?

 

Peter E.,

this one has an Yasnak LX3 control. Did you send Mastercam to it? What post processor did you use?

There are 20 or so files in the .tl8 library. They mostly begin with L but there isn't one with MM in it. There is a Ltools.tl8 and a Ltoolsm.tl8 . The file name is in lower case in the library, when I select it in the pull down menu it goes to upper case. I have selected Ltoolsm.tl8

 

Peter E. & Chris M.,

Do you guys mean never ever use TNR comp, or just use it in the computer and not in the control? I presume the lead in/out is for the TNR comp to be applied.

 

Jim,

Sounds really good, how soon can you organise this?

 

Jadkins,

thanks for the rap on the machine. We need some encouragement. Can you expand a little on the lead in/out values direction, please? Ours has a Yasnak LX3 too. What post processor do you use? Is there one in the V8 mastercam library that will work?

 

Thanks a lot for your time on this everyone, I really appreciate it.

Hugh.

[chris m]

quote:

---

Peter E. & Chris M.,

Do you guys mean never ever use TNR comp, or just use it in the computer and not in the control? I presume the lead in/out is for the TNR comp to be applied.

---

I mean don't use TNR in the CNC; let the computer [or your pencil and paper] do it. If you stay away from G41/G42 you have a much better handle on what the machine is actually going to do when it reads your code. In milling, some cutter compensation is a must for finishing; typically not so for turning. If the insert radius is .020 instead of .0156 it is typically not the end of the world. The main reason people get into TNR programming is that they use "blueprint" numbers in the programs and don't want to figure out the adjustments for radius values. If you are using MC, let it figure out the comp and you will have much better control over the machine's movements.

 

The lead in and lead out are to keep you from rapiding into or out of the piece; feed is what you need

 

C

[Hugh.Venables]

Thanks Chris. Really appreciate your time.

Hugh.

[chris m]

My pleasure

 

What goes around comes around; I going fishing for help out here all of the time.

 

I'm just glad to be able to give advice once in a while instead of just asking for it all of the time!