Dealing with slugs

[M. Roberts]

People, I hope all is well. I have a occurring job which involves wire EDMing a 16.5mm OD x 10.5mm ID x 100mm tall tubes from a block. I EDM drill the starter holes for the ID of the parts. My current method as stated, is/was to pop in the starter hole, wire out the ID, leaving a tab to hold the core, cutting the wire, and jumping to the OD, and cutting it; then when the OD was done, snap out the ID core. This is leaving an undesirable burr on the ID that I would like to make better. Yes, I could break the core out prior to doing the OD, but that would really throw a wrench into the desire to run "lights out".
I had the thought of cutting the ID complete, cutting the wire, rapiding out of the way (in this case, the Y+ direction), letting the core fall, then index over to the next starter hole, and repeat. Part of my issue (I do have issues) is that I cant find the happy medium where the code and the core meet...meaning sure, I can program the ID circle complete, but sometimes the material fractures prior to the completion of the cut, and it shorts out..make sense? Is there a code that if the machine senses a short, it will automatically cut and jump to the next line of code (2003 vintage Sodick AQ750)? Another thought; is it possible, that once the cut is complete, to rapid the Y and V axis separately, and use the upper flushing jet to push the slug out of the cut?

I'm open to ideas!
Thanks, Mark

 

[bigjon61]

How big of a start hole can you start with? If you can get it to .375", use a slugless machining technique. Take 1 rough pass, which would turn the slug into start, and a skim pass to finish the size if required. You could probably get it dialed in to just take the one pass though. Hop to the OD and cut the outside profile.

 

[RJT]

You will need a start hole for the ID and one for the OD. Rough pass the ID, leave a tab, cut the wire, rough the OD, leave a tab, cut the wire, move to the next part ID and repeat. When you can attend the machine, go back and cut the ID tab, remove the slug, skim finish the ID, cut wire, skim finish the OD, cut off the OD tab. If you cant remove the tab on the OD with some other method, make a fixture to hold 75% of the OD and skim the tab. That's the best method I have come up with to deal with lights out wire work.

 

[implmex]

Hi M.Roberts:
I've had really bad results trying to rapid away from a slug...it will occasionally catch in the lower flush cup and rip it to shreds, never mind shifting the job on the table.
I really like bigjon61's method in post #2...yeah you might have to run one or two skims to get it accurate, but it's safe and foolproof.

Your bore is not very big, so a skim is not that much of a sacrifice in time and wire.
In my experience you kinda need it because the asymmetric flushing pressure tends to push the wire away and make the bore too small if you've taken out most of it with a drill.

I recognize that putting the block up on the mill to rough the bore in is more of a pain than putting the block only on the hole popper and popping two start holes, especially if the block is already hardened or is made of some undrillable shit.
If it is super unattractive to do bigjon's method, then I'd do it like RJT recommends and accept that you'll have to tab all the ID's when you arrive in the morning.

Trying to flip out a slug reliably with high lower flush pressure is pretty unlikely in my experience.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[JZ.]

People, I hope all is well. I have a occurring job which involves wire EDMing a 16.5mm OD x 10.5mm ID x 100mm tall tubes from a block. I EDM drill the starter holes for the ID of the parts. My current method as stated, is/was to pop in the starter hole, wire out the ID, leaving a tab to hold the core, cutting the wire, and jumping to the OD, and cutting it; then when the OD was done, snap out the ID core. This is leaving an undesirable burr on the ID that I would like to make better. Yes, I could break the core out prior to doing the OD, but that would really throw a wrench into the desire to run "lights out".
I had the thought of cutting the ID complete, cutting the wire, rapiding out of the way (in this case, the Y+ direction), letting the core fall, then index over to the next starter hole, and repeat. Part of my issue (I do have issues) is that I cant find the happy medium where the code and the core meet...meaning sure, I can program the ID circle complete, but sometimes the material fractures prior to the completion of the cut, and it shorts out..make sense? Is there a code that if the machine senses a short, it will automatically cut and jump to the next line of code (2003 vintage Sodick AQ750)? Another thought; is it possible, that once the cut is complete, to rapid the Y and V axis separately, and use the upper flushing jet to push the slug out of the cut?

I'm open to ideas!
Thanks, Mark

What kind of tolerance are you looking for? Also what are the allowed conditions of the OD finish?

If you are cutting these out of a block and have 2 start holes, I would no-core and finish all the ID's first then I would rough and finsih the OD's only leaving like a .030in tab. Obviously your OD is going to have a spot from the tab, so if its acceptable to file/blend in it shouldn't be to bad. If you have to cut the OD and ID with no witness marks from a tab, id be looking into making them out of round stock and just doing the ID.

I would def try to stay away from making any rapid moves with the slug floating around in there causing a short-circuit.

 

[implmex]

Hi jz814:
I've become disenchanted with the quantity of wire used and the time it takes to no-core cut something as big as a 10.5 mm bore.
At a stepover of about 0.012: it's a long long process in a 4" tall block.

Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[JZ.]

Hi jz814:
I've become disenchanted with the quantity of wire used and the time it takes to no-core cut something as big as a 10.5 mm bore.
At a stepover of about 0.012: it's a long long process in a 4" tall block.

Cheers
Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Oh for sure I agreee its going to take some time and use a bit of wire, but if you can get a good size start hole in you can start from that ID and step out from there cutting down on a ton of cutting time ,still going to take some time but if you want lights out machining you have to compensate somewhere. I typically do a .005 to .008 step over when I no-core, I get what I consider a decent feed rate in 4in thick parts, right around .100in/min or so.

Other than tabbing both the ID and OD then coming back to cut them off, how do you run lights out on something like that?

 

[Luke.kerbey]

I would personally tag the ID, and leave two tags on the OD, then come back and cut/ tag Skim the ID, then cut/ tag skim one tag, then drop out on the last OD tag.

 

[Madco]

The Burr is probably caused because of stress in your stock material, when you are cutting the OD the stress in the material comes out so your part is slightly shifting causing the burr after cutting out the slug.
What is the concentric allowance between the ID and OD?
Most ideal would be to pre-drill the hole so you have no slug on the ID at all, without the need of pocketing

Otherwise, if you don't want to pre-drill, i would start with the OD, leave a tab of +/- 2mm, then cut the ID until the tab.
Jump to next part etc.
Then when you come back cut-out the slug with a 1mm overlap, and then cut the tab on the OD at last

Depending of the type of your machine, do you keep in mind some machines do "work" a bit between warm and cold?

I hope it's clear what i mean, English is not my main-language

 

[plastikdreams]

Make a cut across the slug first, then when you cut it out the halfs will fall out much easier than a full slug. Then run a quick skim pass to clean the parting bumps.

 

[M. Roberts]

Guys, Thanks to all for the input. The material is a silicon carbide based ceramic, and the starter hole for the ID needs to be popped in via hole popper EDM; it cannot be drilled...each starter hole thru the 4" length takes about 1/2 an hour. The largest electrode for my machine is 6mm, so I can't take the ID to size. As mentioned, I do pop in a starter hole for the center core, but I do come from the edge for the OD cut. The tolerances are not super tight, but I want to get them closer to size, to streamline the ID/OD grinding operations that follow. I like the idea of cutting the slug in half...I will put some thought on that one.
I did try cutting the ID, and letting the core fall; when it fell, it touched the lower head, thus shorting it out...back to the drawing board....maybe I could make a plastic (non conductive) ramp to go over the metal part of the lower head that would allow the slug to fall out, but not touch the metal shorting it out...IDK, just thinking...
Mark

 

[OffsetLeft]

There's more than one way to skin a cat, but trying to drop a 10mm x 100mm slug unattended just isn't a good idea, IMHO.

You'd be far better off to pop a series of start holes, 20 or so mm apart, make your program according to that spacing so that it roughs all the IDs to a tab, one after the other, then come in from the outside and rough a profile that includes all the ODs and their tabs up to a stop that keeps the outer slug in place.

Hit start and go home.

Next morning, cut through the tab for the outer slug, cut all the ID slugs free, and it's 'Off to the Races!' running whatever skims you need to run. (If this is a 'rough cut to size' type of operation, just make sure your slug cutoff program extends past the glue tab, so that once you've pulled the slug and brought the upper guide back down, there's still some cutting happening to blend out that 'burr')

Finally, cut each tube free of the block and all you've got left is to finish the cutoff area.