What's new
What's new

May need a custom drill/cutter for phenolic

macgyver

Stainless
Joined
Aug 2, 2012
Location
Pittsburg, KS
Hey guys, I am quoting a job that may turn into alot, I am drilling/routing holes in 1/2" thick phenolic. The hole is stepped, 1/4" through, 1/2" counterbore 3/8" deep, then a 1" counterbore 1/8" deep to finish it off. It is for hundreds of holes per part and the customer hopes it turns into lots of parts.

So, my thought is if it goes into production, does anyone think I could get a drill made to do it in one op? The sample material he gave me looks like the canvas or linen phenolic.

Thanks,
Jason
 
The problem I see is that the 1/4 is going to wear much faster than the others. the dull tool will make a messy burr o n the backside

I would do it all with a 1/4 carbide tool and gain time by multiple fixturing
 
gustafson -

not an argument, I don't have a cnc. But on a pin router I would expect the opposite, the largest C-bore "might" wear faster than the 1/4" carbide drill in the center. Though that is somewhat speculative, my pin-router runs about fast (10K rpm)enough to use carbide or stellite wings on the C-bores, but maybe not really ideal fast speed for a 1/4" carbide drill.

Please explain why the opposite might occur.

Thanks!
smt
 
I can change rpm on the spindle, but not sure if it can change quick enough to do it during the drill op, and pausing it to change rpm would take away the speed advantage I am looking for.
I ran it last night with 3 tools to experiment and I am OK with the results, but I have not ran it with a single 1/4" yet to get a time comparison, it may be right at the same as the 3 tool combo.
 
I'm just starting with cnc, total amateur!

But, if I understand, the options are to get a double stepped drill/counterbore custom made, or drill w/ 1/4" mill and interpolate the 2 counterbores, yes?

Or is the alternative 3 separate tools - 1/4", 1/2", 1"?

Seems to me the custom tool would be quickest of course, but WAY more expensive to purchase & resharpen than a whole bunch of 1/4" mills. Changing tools has to be WAY slower than interpolating.

Just my 2 cents, from a guy who has just enuf knowledge to be dangerous
 
gustafson -

not an argument, I don't have a cnc. But on a pin router I would expect the opposite,


smt



the smallest diameter does more work as it pilots the entire depth where the other steps have no center cutting and work to a fraction of the depth

If you over drove the spindle speed to make it perfect for the 1/4 you would wear the larger, but you wouldn't do that cause it would chatter like crazy
 
I can change rpm on the spindle, but not sure if it can change quick enough to do it during the drill op, and pausing it to change rpm would take away the speed advantage I am looking for.
I ran it last night with 3 tools to experiment and I am OK with the results, but I have not ran it with a single 1/4" yet to get a time comparison, it may be right at the same as the 3 tool combo.

would depend on time to change tools

what machine are you running on?

I figure if I was doing it on a machine with 10k spindle 10 parts on the table, 2 tools it would take around 12-15 seconds a part.

drill with a 3/16 carbide, interpolate the rest with a 1/4 end mill

reason for the drill is as the end mill gets a little bit worn it blows out the back for an ugly burr. done this way you could run the tools till they drop and still have a neat part
 
It will be on a multi spindle Komo cnc router, so actual tool change times on my machine are very quick as they are already there along for the ride, just have to retract current tool/spindle, then drop new one and turn on. If I am running it at 18K, then it does take a short time to get up to speed, but nothing like swapping tools in a single spindle machine, especially if it is a 12ft bed machine and has to go all the way back home to get it.

If I were to run 3 separate tools like I did on the test, I'd still run all holes with one tool before switching to the next.

To be honest, I will probably do the pilot drill and finish it with a 1/4" router bit. It is just one of those things that if it turns into thousands of holes, it may be worth a custom tool. My test I ran all 3 tools at the same rpm to see what it would do. Good results on all three. The 1/4" drill I used is a carbide tipped spur bit used commonly in pt to pt machines for dowel holes or shelf pin holes. I was able to plunge one shot, no peck at 2500 rpm and 100 ipm. Not sure as to long term use without a peck cycle, but I bet it would be fine. It pulled a nice chip, not alot of dust.

It will be backed up on a spoil board so blow out should be minimized if any.

Richard, there are a few options, I can do the custom tool, make it one shot per hole, or I can use a combination of tools. If I do the pilot drill, I may use the current 1/4" drill, then a 1/2" router bit, then interpolate the 1" with it. Would save a little bit of time by just plunging or drilling the 1/2" step and then it could interpolate in one pass vs a couple for the 1/4" as I am sure it would leave a thread of a burr to get rid of if I only did one pass around the 1" counterbore with the 1/4" bit.
 
Is helical interpolation possible with this control?

If so, a bit/EM slightly under 1/4" could finish all three holes, more quickly than drill/plunge/pocket and save some tool change time. A short, stiff tool (LOC slightly over 1/4") that does the upper pocket, then the mid, then the through hole could take better advantage of the spindle speed than a longer floppier tool.

Is chamfering the holes necessary?
 
can you spin the spindle faster?

doing the hole thing with one tool just seems so much faster than the compromises required on a 3 diameter tool, with zero costs and no worry of breakage
 
I have had many occasions to bore similar size holes, in wood for perimeter wood edging on work benches. I got tired of boring 7/16" thru holes and then replacing the drill with 1-1/8" Forstner bits.
I took a 1-1/8 " spade bit , rough trimmed it to about 1/2" diameter and left 5/16" of original size at shank end. Then ground and honed to 7/16" for thru hole. Took about 1-1/2 hours. Used a Dremel tool to rough cut the bit.
This worked very well for me and saved a lot of time. I do know that a spade bit will cut nicely thru some plastics like Plexiglas.
 
I finally got the go ahead and ran one part today, did a 48 x 84" top it has 429 holes for inserts in it plus 2 mounting holes per to screw the insert in. Took all afternoon to run. I ended up running a 1/4 drill through then interpolated the 2 counter bores with a 3/8 downshear. I think I will mess with it some more to get the cycle time down.
I am running into a problem with the material being wavy - nonuniform thickness and of course the customer wants the inserts to be held pretty tight to just under flush. I ran an indicator across it and I saw up to 0.030" difference.
I am back to considering a floating head that I was discussing last July.....
 








 
Back
Top