Official Luthiers Forum!

As a companion to my indexing thread, I'm looking for some advice on how to drill very accurately positioned holes in my table. I'm planning on 1/4" holes using 1/4" dowel pins for indexing.

I have at my disposal:

A large center drill like this: http://www.google.com/products/catalog? ... ps-sellers

My center drills are labeled F1 & F2.

Standard length split point drill bit. Length of the flutes is about 2-3/4" (long!)

1/4" end mill.

I could also buy a stub length 1/4" drill bit for added rigidity.

My plan was to drill with the center drill first and follow up with the 1/4" bit. The questions are:

How deep should I drill with the center drill?

Will the 1/4" bit end up where I want it to be? Position is pretty critical in this application.

What size dowel pin should I buy to get a tight but removable fit?

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Personally, if the placement and fit of these is critical then I'd not drill them but rather, interpolate these holes. Forgive me if you know this already but interpolating a hole means to create it with a contour operation by walking a smaller end mill around and down in order to produce the hole. In this case a 3/16" end mill will work.

Interpolating these holes will accomplish two things:

1. Spot drilling and following up with a 1/4" drill will work fine with any homogenous material....but if there was grain involved (probably not - but if there was) even though the spot placement will generally be perfect, the 1/4" might be forced to walk because of the grain. Interpolating the holes takes all manner of bias in the material out of play.

2. Any holes created by interpolation can be sized to fit the dowel. Rather than having to select the proper drill to create a fit, interpolating a hole allows you to program the size of the hole. Typically, I'll measure the dowel and program the hole to be undersized and then sneak up to the fit by making progressively larger diameter cuts until the fit is achieved. Once you know, for instance that with that tool chucked up in that holder, that the right diameter is .2515", for instance, then you can cut all the holes at that size, provided the dowels are consistant.

Lastly, I find it far simpler to spot and drill holes using a simple "spotting drill" (pictured on the link you supplied on the bottom). Centering drills don't do much for me. As a tool for creating a countersink for a wood screw and a drill hole they are still harder for me to use than a simple 90 degree spot drill and a following drill. Easier to figure depths.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Or if you can't (or don't wish to) interpolate a hole, use a drill about .007 smaller than the size you're after and follow that with the proper size multi-flute reamer. Contrary to popular opinion, drill bits usually do not drill accurate (or even round) holes. A reamer can produce one by taking out a small amount to finish the hole. Reamers are stiffer than a drill bit, and due to their multiple flutes, produce a nicer finish in the hole. Think of the difference between using a file versus using a scraper for finishing wood. The file does the hard work fastest, but the scraper shows off the grain to the best effect.

_________________
"Act your age, not your shoe size" - Prince

I think I'm going to try the interpolation in some wood and then in some scrap Al to see how it works but dang it, I just ordered a couple of end mills and wouldn't you know it, they arrived today. Would have cost me $6 to add a 3/16" but now it's closer to $12 when you include shipping.

I do have 1/8" laying around though. Do you think those would flex to much.

Lastly, I was thinking about doing the code for this by hand to ensure that the holes are exactly where I want them but, I imagine that interpolation is a bit more difficult to program than simple G81s or G83s. I haven't looked deeply into circular interpolation but it looks like G02 is it? Anyone know of a good website that describes how to use it?

I suppose I could also make my plan in CAD using my home position as the origin and use my CAM software to hook it up. I imagine that should work just as well eh? Just makes me all nervous you know?

Finally, one other option I have is to ditch the Al T-slot table for a while and replace with MDF for a few months while I get comfey with everything and try my plan in that minus the part where I drill through holes into the profile of the machine.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

+1 for the interpolated holes. It gives you much better control over how tightly the index pins fit.

Dave

I've been using a piece of 1" thick "Starboard" plastic as a table top--I have a grid of holes drilled in it with threaded inserts underneath. I use these holes both as clamping points and as index holes for jigs--works very well. It would be very easy to fasten a similar top down to the T-slot table without having to actually "ditch" the aluminum top.

I have a bigger XZero Raptor that is supposed to ship soon coming along with a T Slot table--my plans are to drill a single center hole (I use the center of X and Y travel as my home position) so that I can index jigs to the table while gaining the flexibility of a T Slot table for non-indexed setups. We'll just see how that goes. I really do like the way that my Starboard table has worked out, and I might end up using it on top of the T Slot table whenever I'm using fixtures that I've already built.

Dave

What method are you using to sneak up on the size of the hole? Tool wear compensation? Something else? I think we may have covered this once but I don't remember what the answer was.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Andy,
Probably the easiest way to get the holes in the right place is to drill the holes to a 7/32 size (undersize) and then finish the holes to the 1/4 size using a 1/4 endmill. This process should give you good true position on the holes. If you want to make sure the holes are round and a very close tolerance in size you will probably want to finish the holes with a quality reeming operation. However, the best way to use a reemer is to have a floating holder that will allow the reemer to follow the hole. If you reem you will need to interpolate the holes prior to reeming or using an undersize endmill to leave about .010 stock for reeming. I have used this process on very accurate CNC machines for my day job and verified results with a CMM machine. The results are usually a function of the accuracy and capability of your machine and your ability to hold other variables constant.

Good luck!

_________________
Brad
Avon, OH

I'm not Zlurgh, but in my case, I just start adding a few thousandths at a time to the size of the hole until it fits the way I want it to. Nothing scientific at all--just the good old empirical trial and error method. I use scrap material to test in, go until it's a little too far and then back off.

Dave

On the Haas controller you can manually add or subtract compensation but then you have to remember to put it back when you're done. When making fits I alway draw the basic contour so it undercuts by a few thou and then draw and bunch of subsequent paths at full depth that progressively enlarge the hole by .00025"R. When it all gets out to the machine I just keep checking between each cut until the fit is achieved. In Mastercam this is real easy to do but it may be more practical to do it via compensation if your software doesn't make this easy. Something to remember....if you want to program all those compensation cuts have the retract be high enough between these cuts to be able to get the pin in there to check it. Could be this idea doesn't work at all with gantry style machines that have limited z-motion.

G02 is interpolation motion - clockwise. G03 is interpolation motion counter-clockwise. If you hand write this use counter-clockwise interpolation because that will produce a climbing cut since the tool is turning clockwise....better for this cut....the tool will stay sharper longer.

I'd always prefer to interpolate the hole with a 3/16" EM for a .25 hole. but 1/8" will certainly work too. The hole depth will matter. If the hole is 1/2" deep for instance, you might want to run the tool around a number of times for each cut. That's a good idea also....to pre-drill the hole with a slightly undersized drill if you wnat to use that 1/8" EM to create the finished diameter. That will take a great deal of stress off the 1/8" EM.

Do you have coolant? Compressed air might be enough but you should plan on using a squirt bottle and programming so the tool retracts between depths so you can stop, clear out chips, and cool if needs be.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Guys, I'm all for the circular milling on a precision metalworking machine tool but not so sure on a CNC router.
Depending, of course, on positioning accuracy of the machine as well as the alignment of the X and Y axes etc.
Any backlash in the screw(s) will produce something other than a true circular tool path unless precision backlash compensation comes "into play".
I would probably choose a 1/4" endmill that has been resharpened on the periphery to a few thou under nominal and then the .250 reamer.
More than one way to skin the proverbial cat, of course. (Poor kitty)
Nelson

Guys.... you are making this too hard!
Drill it, ream it, DONE!

It's a dang HOLE!

Take it from the old tool and die maker - save all the fancy footwork for the places that merit it.

_________________
"Act your age, not your shoe size" - Prince

On 'one' shot holes I use spotting drills like the one Stewart noticed on your link and peck drill. The first peck is also at a very slow feed rate to mitigate walking. Drill and ream is another option, but a spotting drill saves a tool change and avoids problems where the pre-ream drill wandered.

Interpolation can be a mixed bag depending on how well set up a machine is and how good the control is. The old control on my Fadal didn't interpolate extremely accurately, but my new control does. Even so, it's a last resort for holes that I can't bore. I wouldn't count on an interpolated hole having any sort of roundness or accuracy on a router.

(Now that I have a boring head, I don't know how I lived without it...)

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Thanks for all of the advice guys: you've now thoroughly scared me into not drilling my t-slot table just yet.

Step 1, I'm going to go out and find a 1/4-inch spot drill and buy the dowels so that I have something to work with. Depending on how much they cost, I might just pick up a reamer and appropriately sized drill as well.

Step 2, I'm going to play around with the interpolation and see how round it is. I'll do experiments in both wood and some scrap Al if I can find some.

Step 3, Depending on how things go, I might either go ahead and drill into my t-slot table or I might replace it at least temporarily with an MDF top just to prove to myself that I'm doing the right thing.

I think though that if I can get this to work, it should make for super easy zeroing of fixtures and hence parts.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

By the way, I got some interesting links from another site posting this same quesiton:

http://www.ihcnc.com/pages/mill-tips.php

http://www.cnccookbook.com/MTMillFixturePlate.htm

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I thought I'd post on what I ended up doing just so that the discussion is complete. I think that eventually I will pin my table and perhaps even my machine but for now, I'm going with this until I have a few more months of CNC under my belt.

What I ended up doing was making an MDF fence with some relief for sawdust to fall off. I didn't make the "table" portion very wide so that I can still access my T-slots. The idea is that for pieces wider than the MDF portion, I'll just add spacers from the same sheet of MDF underneath. If I need access for a t-slot I can simply leave a gap between pieces of MDF.

What I did was bolt down the "table" portion and then use a pen to plot the location of my fence pieces. Once plotted, I glued and screwed down the fence close but over the line and came back with an end mill to give an X&Y that's perfectly aligned with my machine (unless I remove the fixture of course).

I offset the fence by 1/2" from X0 and Y0 mostly so that I could machine that little hole at XY0 but now that I'm thinking about it, I could just as easily leave a gap in the fences and have the fence at true XY0.

The plus of having a 1/2" offset is that for parts that need the tool to go into the "negatives" to machine a feature I'm already all set (so long as it doesn't go down into my fence!).

For pieces that will require machining all the way to the bottom, I'm going to use some 1" jo blocks that I have laying around to use as spacers. Once the piece is clamped, I'll yank the blocks.

Like I said, I think that a pin matrix would still be better but to not have to re-do things I'd like to think on it a while longer while I figure things out.

Comments are welcome and encouraged.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com