Negative stock cannot be less than corner radius

[ngkim]

After Ver 6.0 i noticed that whenever we select an endmill(flat) cutter for surface machining with a negative stock to leave on drive surface,there will be a warning "Negative stock magnitude cannot exceed more than tool corner radius,it will be reset".i wonder how can i machine a copper electrode with spark gap?kindly hoped someone could help me.thanks

[Rekd™]

Couple options here, best way would be to get the trode with spark gap already applied, then you could use 0 stock. Problem here is getting it scaled properly, depending on the CAD software being used to create it.

Another way, but you'll need to be careful of the Z depths, is to create a new tool with the spark gap applied to the dia.

Hope this helps

Rekd

[This message has been edited by Rekd (edited 04-02-2001).]

[Mark H]

This is what I do for cutting electrodes with "negative stock to leave"...

For the finish passes I always use ballmills for the 3D surfacing. And if I do need to use a flat endmill I will see if a 2D toolpath will work. With the 2D toolpath make sure both "XY stock to leave" and "Z stock to leave" are set to the same value.

[This message has been edited by Mark H (edited 04-02-2001).]

[Henry]

Rekd,scaling is no option for spark gap.

1.If you use negative stock,then use only ball endmills or bull mill with corner radius atleast same as spark gap.

2.Stock size zero,but subtract 2gaps sizes from endmill diameter and gap from radius.Only drawback is that on 45° degree walls you get slight distortion,if you use flat endmills.

 

[Rekd™]

Henry,

Scaling the model to the size of the electrode's spark gap has worked for me on all but the most complex or obscure trodes when I was in a mold shop. If you have an engineer that knows how an EDM works, it should not be a problem.

Rekd

[ngkim]

but i wonder why before Ver 6.0 everything was okay even with negative stock for flat endmills!?

[Allan Brown]

Allowing us to do something in MC and actually doing it correctly are two different things. This was the case in V6.

I'm under the impression that limiting the tool types and allowable amount of negative stock left are both limitations of the mathemagics involved and the potential for disaster in some scenarios.

[Guest CNC Apps Guy 1]

Allow me to pose this question to those who need/desire this feature.

If you have a sharp corner and you wish to go negative into a surface, where do you calculate the tangency point from? "The center line of the tool" you say? What about comping for the diameter. The tool will will be shallow in some areas and deep in others. "The sharp corner of the tool you say"? That's fine if you're on a wall with some draft, but what if you're on a floor with some angle to it? Then where should the tool coMp from? A tangency point is what is required to do this correctly, and to have a tangency point some amount of radius is needed.

That's my understanding of the reasons why Mastercam does not do that. If I'm wrong, please enlighten me.

------------------

James Meyette

[Trevor Bailey]

Well Put James.

------------------

Trevor Bailey

[email protected]

Specializing in Contract Programming

[Henry]

James,

Mastercam's competitor,Alphacam and specially Sandy Livingstone declared in alt.machines.cnc that it is possible.I'm not getting too much into this since my English isn't that good.Someone should write an illustrated story what's possible and what's not.

[Guest CNC Apps Guy 1]

Henry,

I'm not saying it's impossible, I just posed a few questions about it. I (more or less)was wondering out loud about some of the mathematical aspects of this challenge.

Has anyone ever tested(by physical measurement) the competitor's claim that they can do it. Sorry but I'm a skeptic by nature. "You gotta show me".

Believe it or not, some CAD/CAM companies go through Mastercam's functionality list to do something that Mastercam does not, in many instances it is not a necessary feature but rather a marketing ploy just to be able to say "We can do it and they cannot".

Mastercam continues to develop it's highly successful software by adding features continually, though sometimes not as fast as we(Resellers) would like(What do you mean we can't have it now?????? )! Writing software, when you look at what all is taking place, is a pretty delicate process and it takes time. So with that said, I'll continue to wait anxiously(sp?) for what is cooming through the pipeline soon and not so soon).