surface machining and DNC

[Bob W.]

I have been asked to bid on a job that involves a significant amount of surfacing and I would like to give it a shot. The part is about the size and shape of a laptop computer lid and it requires a nice finish but it will not be a cosmetic model. I have a few questions...

 

If I machine the surface with a parallel tool path (finishing) and a .25" ball mill what feed and step over would you recommend with a 6000 rpm spindle?

 

Also, I need to get set up to run the mill via DNC and I am not currently setup for this (floppy drive). What do I need to get to be able to run DNC? Will MasterCAM do it (Level 3) or do I need third party software? Any special cables required? Is it easy to set up?

 

Thanks,

Bob

[Bob W.]

Also, I should mention that the mill is a Haas

[Flycut]

How old is it?

[Chris Rizzo]

About the only thing you'll need is an rs-232 cable. You can build one yourself from radio shack stuff, however I recommend giving the folks at Preadator a call and getting one of their nice cables. They are out in Beverton.

 

The Mastercam editor will dnc just fine for you. A little bit of setup and parameter setting in both your computer and control. What year is your haas control? I all run ours at 115,xxx baud. set control to dc codes.

 

What's the material your cutting?

[Colin Gilchrist]

+1 on the Predator cable. It doesn't get any easier. The cable is tripple shielded against electrical interference, and you buy a pre-configured "Plug end" for your Haas and a plug end for your serial port on your computer. Just plug everything in and DNC away...

 

HTH,

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[camgeneration]

edit: never mind, I type too slow.

[Bob W.]

The mill is a Mini Mill and it was new in November 2005.

[Bob W.]

I will be cutting aluminum. Any info on the speeds and feeds with the ball end mills?

 

Thanks,

Bob

[sharles]

It's hard to say without knowing what stock you'll have left at this point. First I might suggest getting away from parallel toolpaths. I have moved to the scallop toolpath more and more because I don't have to deal with the large "scallops" that the parallel toolpath will leave on a part with complex shapes. Maybe this shape is simple enough to use the parallel toolpath.

 

As for speeds and feeds you ought to be able to crank it pretty high. At 6,000 you ought to be able to run 200-300 ipm minimum, stepover approx. .015-.03 again depending on your finish requirements. .015 will look good (not perfect). .03 will be fairly coarse.

[Bryan Johnson]

Assuming that you can keep you file size to 1.4 MB, you can DNC from the floppy drive, and would not need the cable.

 

Haas control without the high speed option. I would not expect to exceed 80 IPM before running into jerky motion. The length of each move also has a lot to do with this.

[chris m]

6000 RPM surfacing in Aluminum is going to suck, in general, but what're you going to do? I would consider a speed increaser but there isn't a whole lot of room in a Mini Mill so you're probably SOL there. Haas used to have a feature in their control where you could 'test drive' certain features that you didn't own for a limited amount of time; I would suggest enabling the High Speed Machining option if you can to run this part if you are going over 100 or 150 IPM.

 

C

[Thee Dragracer1951]

+100000

 

 

I have a 2000 minimill an dit will not surface above 80 or 100 ipm. I asked the haas factory about turning on the trial for high speed and they told me that I had allready used it up. I told them I bought it used and they told me that for $2900 they would give me a code

 

So I bought a new Sharp 2412s

 

I have two haas's and thier days on my shop floor are numbered

[tooling]

Depending on what your part looks like parallel might not be the best tool path. If your machine only will run 6000 rpm and 100ipm run it at that. I usually run a .010 step over with .25 ball. mastercam will do a scallope calculation for you also. You should be able to run the cutter at a minimum of 8000 rpm and 200 imp with a ball nose carbide inserted cutter. My machine spindle is 8000 max. I like to use the contour fallowed by the shallow. Sometimes the parallel is the best option but not at the corners. Post the file and someone will help out.

[Todd Tracey from Fastech]

A Project Blend (V9), or Finish Blend (X) will do a nice job as well

[Chris Rizzo]

Everybody seems to agree the mini-mill is not ideal for this type of job, but that's what you got, and don't fret you can certainly get your job done. I've done many a project like this on our mini-mills because that's all was available at the time too. I got used to hearing "you did this on a mini-mill?? NO WAY". Lord knows I'm not a haas fan either, but when in Rome......

 

Getting your dnc system (and posted code)bullet-proof will allow you to run lights out, which might be needed for the long cycle times of surface toolpaths on a 6000rpm machine.

 

I'm in portland too, e-mail me if you need a hand.

[Bob W.]

So MasterCAM will run the machine directly from the computer, correct? I plan to head over to Predator software and pick up the cable in the next hour or so. Do I need any additional software other than MasterCAM to run the mill DNC? Is the setup very difficult? I have been running all programs to date via the floppy drive.

[jeff]

quote:

---

Do I need any additional software other than MasterCAM to run the mill DNC? Is the setup very difficult?

---

Mcam should be all you need, if you can't get that to work, there are some free demo programs that you can download in a jiffy.

Setup is not hard really.