Enlarge hole in carbide part?

alphonso · Dec 21, 2019

Rather nebulous inquiry made the other day. Potential customer has a carbide part with an 11/32 hole through and wants to open it up to 7/16. Unknown quantity other than it's "steady". What processes are used to to something like this? Grinding? EDM? Best process for short run production?

Don't know if the enlarged hole is just straight thru or if it will need to be radiused to the inside cone.

Milland · Dec 21, 2019

These guys claim to make a diamond coated carbide-cutting endmill:

Introduction of Products :: UNION TOOL CO.

If they still do (the original press I read was around 2013) then it might be an option, but you'd have to check with them as to availability and cost. Aside from that, I'd be using diamond grinding pins. If you go EDM watch for cobalt depletion.

as9100d · Dec 21, 2019

Lathe with an ID grind attachment.

Sent from my Pixel 3 using Tapatalk

johnoder · Dec 21, 2019

Or a Moore jig grinder

michiganbuck · Dec 21, 2019

I think a 5/16 diameter point mounted or arbor mounted resin bond diamond ID wheel use with a wet ID grinder or a jig grinder would/might be considered.
EDM may be good but never did EDM ID grinding.

EDM sinker machines are/may be the way to go. I did a lot of external EDM surface grinding...once set up it was a fair cost.

Again ..never did EDM ID work,
Elox Royale Astra MK II 50S Sinker Type EDM Machine | eBay

Eltee Pulsitron EP30/RDP Sinker Type EDM 208-480V 3Ph W/System 3R Mag Control | eBay

Red James · Dec 21, 2019

Wire EDM ... start hole is already there.

CarbideBob · Dec 21, 2019

Looks to be about .375 though distance and .040 per side in C11 carbide so cold header type stuff. Lot's of cobalt, a bigger grain size and on the very soft side.
Waiting for a wire EDM cut time estimate from those who do it. It may be the best.
Knowing if you need that radius is also very important as the wire won't do that and it will slow down the grind.
This can be done on a mill, lathe, surface grinder or ID grinder. If you have to grind it you will want coolant (water or oil) at this amount of stock removal.
What machines do you have to use that can handle flood coolant?
If wire the best is there volume here to buy a wire if you do not have one?
You can do this on a low end Hass mill or even a Tormach and less.
Bob

alphonso · Dec 23, 2019

CarbideBob said:
Looks to be about .375 though distance and .040 per side in C11 carbide so cold header type stuff. Lot's of cobalt, a bigger grain size and on the very soft side.
Waiting for a wire EDM cut time estimate from those who do it. It may be the best.
Knowing if you need that radius is also very important as the wire won't do that and it will slow down the grind.
This can be done on a mill, lathe, surface grinder or ID grinder. If you have to grind it you will want coolant (water or oil) at this amount of stock removal.
What machines do you have to use that can handle flood coolant?
If wire the best is there volume here to buy a wire if you do not have one?
You can do this on a low end Hass mill or even a Tormach and less.
Bob

All my machines have flood coolant. I don't have any EDM machines, sinker or wire. Not opposed to purchasing such if quantity justifies it.

The link to diamond coated endmills is interesting, would need to get some sort of speeder or spindle for the required 30,000 rpm. I don't think any of my tool post grinders will go that fast.

plastikdreams · Dec 23, 2019

CarbideBob said:
Looks to be about .375 though distance and .040 per side in C11 carbide so cold header type stuff. Lot's of cobalt, a bigger grain size and on the very soft side.
Waiting for a wire EDM cut time estimate from those who do it. It may be the best.
Knowing if you need that radius is also very important as the wire won't do that and it will slow down the grind.
This can be done on a mill, lathe, surface grinder or ID grinder. If you have to grind it you will want coolant (water or oil) at this amount of stock removal.
What machines do you have to use that can handle flood coolant?
If wire the best is there volume here to buy a wire if you do not have one?
You can do this on a low end Hass mill or even a Tormach and less.
Bob

Depends on wire size but based on .012 wire with 1 rough and 2 skim passes I'd say under 1 hour per part.

alphonso · Dec 23, 2019

Just informed that the radius is required. "Thousands of parts". Informant doesn't know batch numbers or expected deliveries.

Milland · Dec 23, 2019

Might be worthwhile to turn it into a two-step operation, roughing to take out the majority of material (somehow), then a diamond plated mandrel with the form on it to finish.

GENERALDISARRAY · Dec 23, 2019

I had a job to sinker edm some 3/16 holes through some carbide once or four times.

It was not enjoyable if I remember right.

Do ANCAs have ID wheels?

CarbideBob · Dec 23, 2019

I thought that rad would be a problem.
So that means custom made grinding pins and a spindle speeder of significant power or auxiliary spindle.

Given that it is quantity I wonder how much the customer will spend before just scraping them and buying new ones made to size?

I'd estimate a 8 to 16 minute grind cycle depending on some things. You will eat up a fair amount of money per hour in grinding pins.
You will want lots of water or oil and do you want this carbide sludge in your normal tank ad machine?
On the SGs we have separate tanks for steel and carbide work,...we hate seeing steel come through the machine, contaminates everything.

Bob

aarongough · Dec 23, 2019

Look up 'adam the machinist' on instagram. He routinely CNC mills carbide on his Mori or HAAS using tooling from Union. Pretty cool process and seems like it might be a good fit in this application.

Instagram link: Adam Demuth (@adam_the_machinist) • Instagram photos and videos

alphonso · Dec 23, 2019

aarongough said:
Look up 'adam the machinist' on instagram. He routinely CNC mills carbide on his Mori or HAAS using tooling from Union. Pretty cool process and seems like it might be a good fit in this application.

Instagram link: Adam Demuth (@adam_the_machinist) • Instagram photos and videos

Can you narrow down where this info is located?

CarbideBob · Dec 23, 2019

aarongough said:
.... He routinely CNC mills carbide on his Mori or HAAS using tooling from Union. ....

For some reason you think all "carbide" alike,
Do your tools for 1018 work so well on D2?
If I can cut. mill and turn my 12L14 certainly I can also do full hard D2 with the same tooling.

I have no idea the end use but a "mil cut" might not have the best working surface left behind. EDMs are bad enough.
The grade is known and high binder so this is more "millable" than your standard insert.
Still, how fast can you mill carbide and you need that custom radius in the cutters you buy.

Why do the parts have the wrong sized hole? If you go through learning and tooling and such for the first few thousand will it keep flowing or will they press to size?

One estimate from the wire side without care for any rad. Under one hour. That seems long to me.
Straight hole run, ignore setup. Wire nuts, how long in this hole with a +/- .001 and rough finish surface finish okay.

Mcgyver · Dec 23, 2019

CarbideBob said:
Given that it is quantity I wonder how much the customer will spend before just scraping them and buying new ones made to size?

thats what struck me.....and its 100 thou of grinding! Wonder what having a custom shape sintered costs in volume?

CarbideBob · Dec 23, 2019

Mcgyver said:
thats what struck me.....and its 100 thou of grinding! Wonder what having a custom shape sintered costs in volume?

A basic die cost about 3-4000. Higher if you need cross press which is for the fancy stuff.
Three is a whole big world called preforms.
Here the carbide part is machined while it is still like chalk. There will be shrink errors so this is done to leave .010/.020 for finish grind.
In this you can get basically anything in carbide.
Bob

alphonso · Dec 23, 2019

CarbideBob said:
For some reason you think all "carbide" alike,
Do your tools for 1018 work so well on D2?
If I can cut. mill and turn my 12L14 certainly I can also do full hard D2 with the same tooling.

I have no idea the end use but a "mil cut" might not have the best working surface left behind. EDMs are bad enough.
The grade is known and high binder so this is more "millable" than your standard insert.
Still, how fast can you mill carbide and you need that custom radius in the cutters you buy.

Why do the parts have the wrong sized hole? If you go through learning and tooling and such for the first few thousand will it keep flowing or will they press to size?

One estimate from the wire side without care for any rad. Under one hour. That seems long to me.
Straight hole run, ignore setup. Wire nuts, how long in this hole with a +/- .001 and rough finish surface finish okay.

I'm not sure if the C 11 on the sample part indicates the grade of carbide. I think it may be their method of identifying the hole size. i.e. 11/32. I say this because when first approached they said they want "open up the hole to 14/32".

I hope to find out more details this afternoon.

CarbideBob · Dec 23, 2019

Mcgyver said:
thats what struck me.....and its 100 thou of grinding! ,,,,,

And would we not all like to have that PO. :}

Enlarge hole in carbide part?

Titanium

Diamond

Stainless

Diamond

Diamond

Stainless

Diamond

Titanium

Diamond

Titanium

Diamond

Hot Rolled

Diamond

Stainless

Titanium

Diamond

Diamond

Diamond

Titanium

Diamond

Similar threads