Cutting a .008 Radius

I'm currently running two Mitsubishi Wire EDMs and ive read on forums online that I am capable of cutting as small as a .006 radius with a .010 wire when my machines error out when loading the program when trying to cut said radius or any radius smaller than .009 with the current accuracy E-PACKs that I would be using, I am aware that i can reduce the offset on the E-PACK low enough for it not to error out and run it but then it conflicts with the accuracy i am looking for in accordance to the other passes to the finish size. Any suggestions on a better way of doing so? I am also aware that i can use smaller wire and guides to achieve the result i am looking for but my boss would prefer not to go that route if I don't have to

You could make the geometry a sharp corner and you will end up with a radius between .005-.006

Sent from my SM-G955U using Tapatalk

In my experience, when I've attempted to cut an inside radius that's equal or nearly equal to the offset, the results are not very good. Regardless of how well the power is managed, it's simply not a "clean" corner. (I'd say: "ragged"... is a better description when looking at it under a microscope).

fwiw...

PM

Ya I agree with precisionmetal . I deal with same situation very Often in regards to management always putting the priority on cutting parts as fast as possible and always trying to cut corners to achieve this.. Bottom line is when accuracy and tolerance matter you just can't cut corners.
It takes 20 mins to change guides and do wire alignment. That machine has great tecs for .008 accuracy Tec. Using .008 wire would only rough a bit slower. But you would or should have perfect radius. Are you using Corner master? There are parameters within the EPAK that can be adjusted for Inside and outside rads.
Good luck.

JTB3 said:

Ya I agree with precisionmetal . I deal with same situation very Often in regards to management always putting the priority on cutting parts as fast as possible and always trying to cut corners to achieve this.. Bottom line is when accuracy and tolerance matter you just can't cut corners.
It takes 20 mins to change guides and do wire alignment. That machine has great tecs for .008 accuracy Tec. Using .008 wire would only rough a bit slower. But you would or should have perfect radius. Are you using Corner master? There are parameters within the EPAK that can be adjusted for Inside and outside rads.
Good luck.

Click to expand...

you can't cut corners. Lol. What error are you getting? Interference check?

JTB3 said:

you can't cut corners. Lol. What error are you getting? Interference check?

Click to expand...

yeah I was using corner master and the error i was getting is the P153 LF ERROR, and as I said I could do all this simply by getting the smaller wire but as i said my boss would prefer me not to have to but i will if it's needed. ill probably end up going with just making it a sharp corner and allow the path to make the radius itself.

Hi bbkellough:
I've had best success programming this kind of stuff by doing as others have recommended and running smaller wire.

Having said that, the best workaround if you don't want to or can't change wire, is to layout a centerline path for each of your wire passes with the correct offset in the geometry to account for the wire radius, the overburn and the next pass allowance.
Then just program a zero offset pass for each of those geometries assigning the proper cutting conditions to each but with zero offset called out.
The roughing pass and maybe the first skim will have no radius in the cad pass geometry

The benefit is that the path is unambiguous for the control...it's going to drive around the contour exactly as written, so it doesn't crap out when the bigger offsets normally applied to the roughing passes are calculated.
The downside is that it's a pain in the ass to write all that code instead of just coding the final contour as a sub and calling it over and over with different offsets like most people normally do.

But it does work, and it works well.

However, Precisionmetal makes the point that the corner will end up kind of boogered a bit, and this is mostly because the radius is so close to the wire rad plus the overburn that the wire is not just burning on the tangent of the wire and the surface; it's burning over a wide part of the wire circumference as it approaches the corner.

So if the rad is truly close tolerance, don't rely on this method...it won't quite get you there.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

bbkellough said:

yeah I was using corner master and the error i was getting is the P153 LF ERROR, and as I said I could do all this simply by getting the smaller wire but as i said my boss would prefer me not to have to but i will if it's needed. ill probably end up going with just making it a sharp corner and allow the path to make the radius itself.

Click to expand...

Pretty sure the p153 LF error is because interference check is on. Turn it off and it should run fine with .010 wire down to .006 rad. Anything less then .006 rad go to smaller wire. Or try what others have mentioned. But that's a lot of programming when you could just change wire within 20 mins.

implmex said:

Then just program a zero offset pass for each of those geometries ...

Click to expand...

Marcus and all....

When teetering on the edge of possibilities given a certain diameter ( or radius ) cutter, it makes no difference whether the application is
lathe, mill, WEDM or anything else.

I for one would never consider any toolpath that isn't to the blueprint.
My "workaround" in the sticky situations is that I write separate programs for the roughing and finish passes.

In this case of .008R, there should be only two separate programs.
In the rouging stage, there is a "sharp" corner, while all skim passes can use real Radii programming and you have the option of just adjusting Wire R to fit.

Below .006R however, one might need to fudge toolpaths and use separate programs for at least Rough, 1st skim and then the same for all other skims.

( yes, I did go through this very same thing recently ... and I did not need .008 wire, only a learning lesson )

Hi Seymour:
I get what you're saying, and I'm not recommending anything like this as a routine way of programming your parts.
However, if done judiciously, it is a workable way of eliminating the bad consequences of letting the control try to calculate offsets when the geometry is right on the edge of what the offsets will allow, such as a very small internal corner or radius.

Something also not touched upon in this thread yet (because the OP is running Mits machines and is looking for a Mits specific solution) is the behaviour of the control when it encounters a conflict of instructions between geometry demands and offset demands.

It seems a Mits will throw an alarm and not permit the burn...my Chmer machine will bowtie the corner and trash the job, and it's not always obvious from the simulation.
So for my machine, the workaround I proposed is the lowest risk option I've found for these kinds of situations.
This is when I can't bring myself to do it properly and just change the frickin' wire as JTB3 advocates.

If you ran a Chmer like mine rather than the machines you have, maybe you'd grow to prefer my solution too: a lot depends on what you perceive to be the greater risk or the greater effort.
I know my way will work, regardless of the machine it's run on, and it's safe so long as you don't screw up the cad geometry because it will follow the commanded path exactly.
It's also easy to implement and will show you graphically where the trouble spots are when you do the CAD layout of the roughing pass .
The shortcomings we've already discussed.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

I had this all of the time. This becomes very nearly impossible when you are programming for a four axis form tool. I finally had to buy Esprit. This program will allow you to program using G40 (instead of G41/42). You simply input your offset values when programming, and the program moves the tool paths for you. Then the machine runs using no offsets from the control. Works great!
I have a new Fanuc wire and it does a very good job in those tight corners. It uses a corner control that the machine control implements. The corners look very good under the microscope.