[Cartierusm]

I'm using my CNC Brideport and it's only been CNCd for a few months and this is the first time I've actually cut anything that needed to be accurate. I have an external DRO brand new that's hooked up so as far as the machine accuracy it's dead on. The cuts come out fine but I'm having problems with hole pockets.

Basically just holes but that are a specific size so I'm cutting them with RhinoCAM Hole Pocketing Function instead of drilling them. I'm cutting holes to fit .25" dowel for a jig. The holes are coming out tapered. Perfectly round as far as I can tell but the top part of the hole is let's say .254" (which is correct size I wanted) but the bottom is way smaller probably about .250-.251". I kept incresing the size in Rhino until the pin fit in a little then I re-ran the Gcode about 4 more times to allow for tool flex as the tool is a 3/16" Endmill.

Any reason this would be happening, below is my Gcode. I mean even if the head was out of tram and sorts it would still make a round hole, albeit at a different angle but a symetrically diameter hole, right?

[idtkid]

Couple things that may help, no guarantees:

If the shank of your bit is thin and your running the RPM of the spindle high, the bit may succom to centrifugal forces product a tapered hole

I didnt open your code, however if your pocketing your hole in multiple Z increments, a small amount of play in your drive system will be unnotticable in the beginning but at the end of your program the dimensions could be a ways off.

Yeah, it cant be tram. It is an interesting problem for sure.

[Cartierusm]

It's a high quality solid carbide 3/16" end mill, 3/16" shank, I'm running it at 3000 rpms. I only have about 1" sticking out. But I don't understand if the top of the hole is bigger and I run the program a few times the bit wouldn't know it's at a different position if it's no longer rubbing the walls of the areas that are already bigger. Same as I just said with the drive system being off.

The centrifigul force stuff, that's pretty funny, hope it's not that LOL.

[HuFlungDung]

It is likely not your nc code. Tip wear tends to have an accumulative effect. If the tool advances by .100 in depth for each pass, it is really only the flutes of the tool near the tip that are taking the brunt of the wear from usage. When they get slightly dulled, then the tool deflects and the sharper flutes further on up have no chance to ever remove what they could remove if the tool was not deflecting.

Rough drill the material out of the hole so as to leave only about .005" to remove with the endmill. Then using a brand new endmill, interpolate the hole at depths of maybe 1/4 to 3/8 inch, removing those last few thousands, going around twice at each level. Consider how little movement is actually going on with a .1875" tool orbiting within a .254" hole. 5 ipm @3000 rpm is too high of a feedrate to actually give the flutes a chance to remove all the material. Because the circumference of the circle is only about .0625*Pi = .19", at 5 ipm your tool is completing one orbit in about 3 seconds. Because you are using about 50 line segments to make an orbit, it is doubtful that the control can force the machine to make each endpoint positively before the next movement begins, so this sort of mushy movement results in what I call 'lazy interpolation', where the machine lags behind the programmed motion. Try 1 ipm and see if it is any better, or indeed, a rounder hole. It is difficult to know how tight your machine really is, and you might actually have a 4 cornered hole at the end of it all. Then, you get a custom reamer to really solve the problem.

[Cartierusm]

Hu, I didn't realize you spoke Chinese, thanks for the lesson..LOL I appreciate the help and do understand what you're saying, but you say interpolate, I understand the concept but not how to do it. I use CAD it does the work for me.

Now after all those compliments I'll get into what I meant to say, it's a brand new end mill picked it up today.

As for the info on IPM that makes sense I'll try that, thanks.

Would the too fast feed rate still be the culprit even though I re-ran the program about 4 times?

[HuFlungDung]

"New cutter" designation only lasts about 1 millisecond, then its a used cutter If you damage the sharp corners by plunging with the tool, it won't cut as you'd hope a new tool would. By rough drilling the core of the hole out, you preserve that delicate stage of 'new' for a few seconds more

Linear arc Interpolation is what your nc code file shows for commands. There are no arc cutting commands in the file, so what you've opted for in RhinoCAM is to simulate true arcs by means of short line segment commands which have an inherent small amount of deviation from the true circular path you intend.

You can always tell if the feedrate is too fast: if a subsequent rerunning of the program removes more material, then the feedrate on the first go round was too fast to permit the tool to remove all the material. Add to that the fact that the machine achieves more perfect motion when moving very slowly because it is getting more positional feedback per command (on a servo system).

Of course moving dead slow is not productive and tends to wear the tool prematurely. But in this case, you do what you have to do, because the chosen process is not the optimal method to do a hole this deep.

In a production setting, one might run a finish cut at a higher feed, and adjust the toolpath (using radius compensation on the machine) to purposely cause the tool to move in an overcut path, knowing full well that something is deflecting, and that the final size will be predictable after running the program a time or two. If you resort to this latter method, then you will indeed spoil the hole if you rerun the program and allow it to take a spring cut, unless you cut the radius compensation back a tad or two.

[djr76]

Hu, I didn't realize you spoke Chinese, thanks for the lesson..LOL I appreciate the help and do understand what you're saying, but you say interpolate, I understand the concept but not how to do it. I use CAD it does the work for me.

Now after all those compliments I'll get into what I meant to say, it's a brand new end mill picked it up today.

As for the info on IPM that makes sense I'll try that, thanks.

Would the too fast feed rate still be the culprit even though I re-ran the program about 4 times?

Circular motion feedrates must be increased (outside) and decreased (inside) then normal linear feedrates .

Linear feedrate = rpm*feedrate per tooth*teeth/flutes

Outside arc feedrate = linear feedrate*(outside radius of part + cutter radius)/outside radius of part

Inside arc feedrate = linear feedrate*(inside radius of part - cutter radius)/ inside radius of part

[Cartierusm]

Ok, so I should start with running it at 1 ipm and see where it gets me. Thanks. I'll try it tomorrow, at least it wasn't anything majorly wrong.

As far as RhinoCAM give short segments to simulate arcs, then what is the alternative, is that only because I'm using a Hole Pocketing function, is there a different function I should be using?

[jimdakotart]

depending on the material you are cutting makes a huge difference, also shorten up tool stick out to barely more then depth of cut (D.O.C.). some times high speed cutters work better for various materials then carbide. also you can utilize. if your machining fiberous material like wood, fiberglass, or prototype material from Goldwest or machinable wax. Check out the guys at Harvey Tool. they make some unique cutters styled for plastics, fiberglass, carbon fiber. If your gonna work with carbon fiber or fiberglass, check out Fiberglast out of Dayton Ohio. also if you are utilizing standard R8 holders get the endmill style where they are more rigid, or get the cash out, get the R8 holder that excepts collets like the ER style. where you keep the 1 tool, but you swap out the collets in the end of the tool holder like commonly found on Cat-40 and Cat-50 holders. Check out Ebay for kicks, or there is a variety of sources to get better ideas, like http://www.usshoptools.com. Give me a hollar if still lost, there is also a lil place here in Cleveland, Ohio called SmallTools you might be able to hitup. My Favorite is source the stuff at tool shops, hit the web n cut costs. Theres a few more options like a adapters for the spindle where it's gearbox that increases the spindle rpm's and the runs like 3x or 4x for higher spindle speeds. but try simple stuff especially air blower for chip removal, vaccuums, air mist coolants or flood coolant or a good old squirt bottle with coolant, also coated tools may help but costs can ad up.. Best of Luck Jim

[davereagan]

This seems like polevaulting over a mouse turd. Why not ream the hole and be done with it? If interpolating is the plan, program by hand:

:G90
G0 G94 X.0625 Y0 Z.1 M3S3000 F.001 H1 M8
G1 Z-.1
G3 X.0625Y0I0J0
G1 Z-.2
G3 X.0625Y0I0J0
G1 Z-.3
G3 X.0625Y0I0J0

etc.

[Cartierusm]

Dave, I like your way with words, but if you didn't notice what I said above I know nothing about coding by hand. Plus my supplier didn't have a reamer that was .252", the catalog didn't even have it, plus why ream when you've got cnc, no need to get a reamer for every operation I ever do, I'd make no money.

[jalessi]

http://tinyurl.com/nraavy

[davereagan]

Thanks. I love the picture I get from that phrase. I thought reamers were made obsolete too when I got my brand new CNC. Then I put some miles on it and all of a sudden, it wasn't holding a tenth or two for hole roundness. LOL. Below is a catalog that stocks reamers almost any size up to 1.000" by the thousandth or even half. Over/under dowel reamers are worth getting atleast for 1/4, 3/8" and
1/2" Reamers and taps will never be made obsolete by thread mills and endmills. Taps and reamers do not deflect inside a hole because they are supported right there on the other side of the hole. A tap will generally get dull and cut dirty threads before it cuts undersized threads. If an endmill or thread mill gets dull, it will push away and you won't know it without measuring. Regarding coding, I bought a machine 10 years ago with conversational programming because I knew nothing of programming and it was a nice bridge. I learned the basic G codes from watching the program run and seeing the code my picture based screens would generate. I made way too big a deal out of it. In under an hour, you could know these basics and not need to hit a CAM station for cutting a circle.

Dave

www.kbctools.com, page 79

[Cartierusm]

Cool, both of you for the reamer info. There is a KBC 20 minutes from me. But as this part just needs holes for location and after cutting out the part the holes will no longer be attached to the piece I'd rather CNC it so as to not waste money. But the over under for dowels for standard sizes does seem pratical, I'll look into it.

But this thread was more like 'why are my holes tapered' not 'how do I get perfect holes' DON'T get me wrong the infor everyone's given me is very valuable and I appreciate it.

For dowels I notice .25" is almost a little too tight for pressing in the dowel for the jig part and it seems as though .251" is about right for a non-wiggle slip fit, but might take a pliers to get out, for the actual work piece. From you guys what are standard dowel size holes for 1/4"?

As for conversational, when I first started I bought the New Fangled Solutions Wizard package for Mach and do use that occasionally. On my CNC lathe I use the wizards all the time, but for the mill I'm so fast as Artcam and Rhino I usually use that. But this part I'm making does have some hole I need to make by hand so I'll be doing those with the mach wizards, but this time I'll pay attention to the code a little more. After a few years of this I do know a little but only enough to make life a little easier jogging around the table.

Smartflix.com has some videos of CNC coding instruction maybe I'll pick up one of those.

[davereagan]

I don't remember if a material thickness or hole depth was menrioned, but if you reamed them .251 and felt the excellent sizing with a standard 1/4" dowel, I think milling a dowel hole would not make sense to you anymore. As far as actual too deflection, high helix endmills help. Short cutters and short holders. Even on this forum, a lot of guys hang their tools out way too far for no good reason. Even on $100k+ machines.

[mc_n_g]

This also depends upon the measurement of your dowel pins. If they are standard precision ground (no coatings) I have always used the standard reamer of -0.0005 (a 0.250" reamer would be 0.2495). The fit is great.
If your pin is coated you need to determine the thickness of the pin with coating. Some chromed pins start at the 0.250 size and then chromed over top adding to the dimension. This means you need to get a decimal reamer to the size you need. For 'onesy-twosy' jobs I have used Wholesale Tools for their decimal reamers if they are not 'normal' sizes.
But I agree if you want to use dowels you cannot mill (or drill) the hole precisely enough. Too much slop and deflection. The reamer is the best way to go.
Also the level of precision you need has a huge impact as to what you do. You see the difference when a dowel jiggles is the hole as compared to a properly reamed hole.
My father-in-law is still frustrated by the fact that if he uses a .375 drill he can precisely locate and drill the hole without other tools! When he goes to align the plates with dowels it does not happen!

[davereagan]

I blew the size on a few holes before I learned a couple of things about reaming. On a 1/4" hole, I'd drill .238 or .242 Drilling the hole too close to size leaves too little stock for the reamer. Also, put an indicator on the reamer and make sure the runout is under
.005" if possible. Here is the most important thing: The length on a jobber reamer is there to let the reamer deflect and compensate for runout and follow the hole. I learned in engineering school if you double the length of a beam or bar, the same force will cause 8 times the deflection. That is a very powerful truth. Runout is proportional to length. So, with a 1/4" reamer about 6 inches long, you get more runout for hanging it out, but for doubling the length it hangs out of the spindle or especially R8 collet, it will only take 1/8 the force to keep it in line. Translation: it will follow the hole without cutting oversize. I made the mistake of choking up on a couple of reamers in my bridgeport for more accuracy and got the opposite. Yes, they had less run out, but they were so stiff, they cut that runout into the hole. Since I've followed these guidelines, I've had good results. Also, don't feed too slowly, or it was cut over as well, especially in the first diameter of depth.

[Cartierusm]

Thanks all good info.

[djr76]

Carbide drills and reamers make pretty straight holes

[Nzoldun]

To make sure a reamer cuts to size, the hole should be drilled ~1/32" undersize and then bored untll ~ 0.012 - 0.020 is left to take out with a machine reamer. The reamer will then be exactly on centre and will not need to deflect at all to follow the hole.