# Milling Circular Arcs By Cnc



## Dave T (Oct 8, 2015)

I have been making fly reels by manual operation of a mill and lathe, and am trying to decide if CNC would also work.
As a new member, it appears that I cannot insert a photo here (because it might be spam?).  But look at my Avatar for an aluminum frame reel, or click on the attached image file to see a bronze frame reel.
Consider the front end ring.  It is a thin ring that is supported by several lugs.  I cut the arcs between the lugs with my mill and a rotary table.  The finish is smooth enough that the part only requires tumbling in stainless steel media to finish.
If I made this part on a CNC mill or router  with X, Y, and Z axes, and used the appropriate G code to cut the arcs, could I achieve the same finish? Or would a rotary table still be needed?


----------



## Karl_T (Oct 8, 2015)

piece of cake on a CNC mill


----------



## JimDawson (Oct 8, 2015)

Welcome to The Hobby Machinist Dave.  We require five posts before allowing content beyond plain text to keep the spam under control, sorry for the inconvenience.

That is a very CNC-able (a new word)  device.  The finish would be a function of the tooling and the rigidity of the machine.  An inexpensive router will be less ridged than your mill.  You could also do the hole pattern on the spool very easily on a CNC also.

Very nice looking reel!
.
.


----------



## kd4gij (Oct 8, 2015)

There was a member here a couple of years ago that makes fly reals an a g0704 converted to cnc. But I haven't seen him on in a while.


----------



## RJSakowski (Oct 8, 2015)

A good CNC will do a very reasonable job of machining a true circle.  There are some small deviations due to lost motion, response time, etc.  When I was shopping for my Tormach, I asked the sales rep. why I needed a boring tool if I had a CNC.  His response was that there will be some inconsistencies and if you want a truly round hole, you will use a boring tool.  That said, I have machined a good many holes using circular pocketing routines and never had any issues with them.

If you can live with .001 to .002" tolerances, A CNC mill should work very well for you.

BTW, Welcome to the group and a very nice fly reel!

Bob


----------



## Dave T (Oct 9, 2015)

Guys,
Thanks for the responses.  What I conclude is that I will probably need a motorized rotary table in addition to X, Y, Z axes.
There is very little in the reel that needs tolerance better than .002, and quite a bit that could be done at .005. What is needed, however, is a smooth, clean appearance on the visible surfaces.  The customers for my reels are guys who make split bamboo fly rods, and they do beautiful work.  They go to great lengths to be sure that no speck of dust gets into the varnish.
If the OD of the front end ring were cut by alternate motions of X and Y as small as .0005, I think that the appearance would be quite flawed, optically.  I would have no choice but to try to fix it with a hand file.  Some guys do nice work with a hand file, but I am not one of them.
Dave


----------



## Karl_T (Oct 9, 2015)

At least for these parts, no need for a motorized RT.

Sounds like finish is critical. This means you need a rigid machine. The very low end machines will likely not meet your needs.

If this is just a business for you, I'd buy the parts from a pro CNC shop. Of course, nearly all of us here want to say, "I made it myself".  In that case, start shopping for CNC mills.


----------



## RJSakowski (Oct 9, 2015)

Dave T said:


> Guys,
> Thanks for the responses.  What I conclude is that I will probably need a motorized rotary table in addition to X, Y, Z axes.
> There is very little in the reel that needs tolerance better than .002, and quite a bit that could be done at .005. What is needed, however, is a smooth, clean appearance on the visible surfaces.  The customers for my reels are guys who make split bamboo fly rods, and they do beautiful work.  They go to great lengths to be sure that no speck of dust gets into the varnish.
> If the OD of the front end ring were cut by alternate motions of X and Y as small as .0005, I think that the appearance would be quite flawed, optically.  I would have no choice but to try to fix it with a hand file.  Some guys do nice work with a hand file, but I am not one of them.
> Dave



A CNC mill does not cut by alternate motions of the x and y axes.  They are running simultaneously at proportional rates to give the required direction of motion.  However, with any milling process, you will have scalloping because of the nature of the cutting action and the tool.  This can be minimized by slowing the feed rate and increasing the rpm for the finishing cut.  The CNC should also run at a constant feed rate so the milling pattern should blend consistently from  the ring feature to the tab features.  A rotary table will not give you that flexibility. 

For good finish, it is hard to beat turning on a lathe though. 

What the CNC mill will do for you is to automate the machining process and the permit machining multiple features in a single part setup, thereby improving registration considerably.  It also will produce identical parts, important in a production environment and allow you to walk away from the process, improving your production efficiency.

Bob


----------



## jeffecc10 (Oct 18, 2015)

Dave what an awesome looking reel. Now I don't know about flimsy cnc. I run cnc lathes and mill every day. The machines we have are very good. So if you have a good cnc mill. You can bring your production of the that awesome fly reel to another level. The contours should be excellent. Beyond that you can produce your reel in a new way. You would need to sit down an rethink your process. Your should be able to reduce the time it takes to make your reel substantially. You would also be able to control your part size an overall quality much better. You can go from one at time to batches at a time and all of them being almost identical. If you don't have a cnc background it would be a good idea to get with someonr that does and go through your reel and come up with a process that wills work well with a cnc. If you have some small cnc shops in your area stop in talk with the owner. A lot of those guys are great and can give you some pointers. Anyway nice reel and good luck



Sent from my Nexus 7 using Tapatalk


----------



## countryguy (Oct 26, 2015)

Very cool project!  I'd love to see how it comes out!  The note on the scalloping is interesting.   Could you use a real small end mill to minimise that?  Say 3/16? or would you go large?     I wonder how these would look from a Plasma CNC cut setup?


----------



## chevydyl (Oct 29, 2015)

I would agree that tooling is key to a great finish, as well as rigidity of your setup and machine. Maybe contact CGS Tool, they can select the proper tool, I use their tools with great success. Plus they are USA made. Add in a profile finish pass of .010 or less as well with high rpm and slow feed. Good luck with it, nice reels


----------



## MontanaAardvark (Oct 31, 2015)

I think the main concept here is taking it from the mill and it's ready to use.  From CNC to dropping it into the reel.  What about finishing with bead blasting or sanding?  The ridges that cutters make on the mill are awful looking but they're physically tiny.  320 grit (that's 320 particles per inch or .0031") should wipe them out, leaving just a grade or two of abrasive to get a really nice finish.  600 grit then 1000?  Or 320 then bead blasting?   

Just don't do it anywhere near the machine; abrasives on the ways are A Bad Thing. 


Bob


----------



## chevydyl (Oct 31, 2015)

Bob, if you reread his post he says that currently all he has to do now is tumble the parts in stainless media and they are ready to go. I bet it will be the same in this case, except for one issue, interpolation circles can show the slightest backlash on your finish, particularly on the 90deg point where direction changes, choosing the correct lead in and lead out can help, I know with my system using a circular lead in/out leaves the best finish for me.

Wow this auto text really did a number.


----------



## MontanaAardvark (Oct 31, 2015)

D'oh!  Sure enough, right at the top.  Sorry about that.


----------



## coolidge (Oct 31, 2015)

I would also look into CAM toolpaths, there are multiple CNC methods of machining a circle. An real industrial CNC mill is going to be WAY more accurate than any manual mill with a rotary table, if you want to hold .0001 you can. That said given these components are round I'd also look at CNC lathes. Modern higher end CNC lathes basically have a multi-axis CNC mill built into them, they drill, tap, and mill from the front, the top, the back, its ridiculous what you can do on one. Of course just one live tooling head tool holder costs $8k


----------



## Dave T (Oct 31, 2015)

I guess that my original question was, how good are CNC motion controllers when it comes to interpolating circles? Perhaps some are better than others. I am considering purchase of the KFLOP controller by Dynomotion.  The CNC mill itself can cause problems if it is not sufficiently rigid, if the ways are not tight, or if the lead screws have backlash.  But the advice that I am seeking has to do with the electronic motion controller.
I recognize that a motion controller does not alternate between X and Y motions but rather coordinates them to occur simultaneously.  Still, I am imagining that there will be a series of "facets" on the largest radius arc, and these will only go away with manual finishing.
The reel back plate is a better item for discussion than the front end ring.  The back plate has many surfaces that I can turn, and I usually finish with 320 and 600 grit, wet.  But the OD with its 5 projecting lugs has to be milled.  I first rough out this shape, leaving about 0.010 inch for the final passes.  The really fiddly part is making all the final arcs meet correctly.   There are 28 arcs in all, 9 are concave and the rest convex. (All concave arcs have radius 0.156 and are cut with a 5/16 end mill.)  There are 18 points of inflection, where a concave arc meets a convex arc, and the part does not look right if these transitions are not tangent and smooth. This is where CNC should be a great time saver.
After turning all surfaces that can be turned, and milling the outer profile with light cuts, I tumble in stainless "jewelers mix".  This tumbling removes all the sharp edges where the mill has cut the outer profile.  It does not greatly change the appearance of the turned surfaces and the milled outer profile.  I rely on manual mill and rotary table rigidity to make a good outer profile surface.
Dave


----------



## JimDawson (Oct 31, 2015)

Dave T said:


> Still, I am imagining that there will be a series of "facets" on the largest radius arc, and these will only go away with manual finishing.



I have never see any evidence of ''faceting'' on any size radius cut with a modern motion controller. You did see this with some of the old NC paper tape machines when they would convert arcs to a series of short lines forty five or so years ago.

Most arc problems today come from mechanical issues rather than the controller.
.
.


----------



## chevydyl (Oct 31, 2015)

On my home built conversion using Mach and bobcad cam there is no evidence Of facets, Even WITH An Adaptive Roughing path it cut very nicely then of course a finish profile pass, the side walls look great, my board is a c62 from cnc4pc and I'm not using a separate motion controller like the smooth stepper. I'm using servos with 2000 line encoders my step resolution is pretty low, like half a tenth or something

I will add that if your getting facets or lines on your walls you need to adjust your feed or rpm, or both to make sure your using the correct chip load. I have a finish end mill 5 flute that wants .0015 ipt feed, equates out to 2200 rpm at 17ipm feed rate. Too little feed causes rubbing, light doc with too slow feed causes rubbing,  light doc and HAUL ASS causes the correct chip load and a good finish....


----------



## chevydyl (Oct 31, 2015)

Also, a tool manufacturer was highly against selling me their bad boy alu end mill because it would cause poor finish cause my machine couldn't keep up


----------



## 09kevin (Oct 31, 2015)

Dave,

I agree with Jim and Chevy, don't think you will have any problems with facets.

Kevin


----------



## Dave T (Nov 1, 2015)

Chevy,
Help me out with your nomenclature:
1. What is "doc"?
2. "ipt" apparently is not "inches per turn" but "inches per flute"?
3. How did you arrive at the .0015 ipt figure for this particular end mill, by trials (experience) or by manufacturer recommendation?
The best ipt is probably dependent on the material; I am using c544 bronze which has a little lead a cuts a lot like brass.
Dave


----------



## Wreck™Wreck (Nov 1, 2015)

The accuracy of an interpolated arc depends on the machine used, the required accuracy and the speed at which one wishes to finish parts. For the work that you are doing a light linear bearing way mill would be an excellent choice, such as the Haas mini mills. Many modern systems can correct for mechanical inaccuracies via software, this may be a bit above the level of money that you are willing to spend as it may require paying someone to do a ball bar test on it.





The finish is also dependent on the speed at which the components must be produced, when you contemplate the prices on high end machines you are paying for not just accuracy but accuracy, speed, repeatability and a long service life. One may make 10 perfectly acceptable parts per day on a less then ideal machine, doing the same at 10 parts per hour is a different thing all together.

Good Luck, your work looks excellent.


----------



## chevydyl (Nov 1, 2015)

Doc, depth of cut
Ipt, inches per tooth
And yes niagara cutter says .0015 ipt feed for the S545 Elite 5fl end mill, it ends up being 17ipm feed rate for a .5 inch 5 flute cutter spinning at 2300 rpm or so.


----------



## chevydyl (Nov 1, 2015)

So I'm not sure that ipt is material dependant, rather cutter dependant, what is gonna cause it to rub? Taking to little doc at too high rpm feeding to slow, so you have to figure out your surface feet, of brass or whatever, so your gonna spin that same endmill 4000 rpm and have a ipt still of .0015, but your gonna need to feed I at 40ipm to keep it from rubbing because of the higher rpm of the cutter. These are just guessing examples nothing is tested just giving an idea. Your going to need to test to see what works.
With my 5fl I fed slow.... terrible finish. The more flutes you have the faster you can feed, and need to feed.
Back to the reel parts, I think it's definitely worth a try, I think you will be pleased with the results, you may even be able to make a jig or fixture that will do 4 or 8 parts at a time and still get the desired finish


----------

