machineing radius edges

Im after a few ideas as its come up recently on another project that zeeflyboy very kindly helped me with but now its come up again.

I am trying to make this part not necessarily all on a cnc but however possible and that will be the easiest and cheapest way for a bit of a test.

basically the bit im stuck on is I want to put a 8mm radius on the edges of a bit of 25mm aluminum stock.

im not sure if my current cnc is going to be up for cutting ali but I could give it a try I guess.


What are my best options/methods?

many thanks

Attachment 22960

If you want 8mm radii and that sharp step in size as in the image you can only do this as a 4 Axis milling job, CNC or Manual.

Radius cutter, however 8mm may be a bit big for anything but a reasonable size machine with a relatively slow spindle.
I've just checked the first cutter I found (arc euro trade), and an 8mm radius cutter is 24mm OD, with 8mm centre, and a 16mm shank, so a failry substantial machine would be needed.

Removing the bulk of material using a normal endmill and several passes would mean minimal cutting for a final finishing cutting pass.

Other option would depend on how good a radius you want. You could probably get a reasonably OK finish using a ball end mill and multiple passes.

But how do you transition from one size to the other with a radius cutter?
I suppose you could clean the transition up with a file?

Quote:

---

Originally Posted by magicniner

But how do you transition from one size to the other with a radius cutter?
I suppose you could clean the transition up with a file?

---

He only asked about the radius edges, not the stepped bit ;-)

It all depends on the quality of finish required.

:highly_amused:

cool wasn't aware you could get something like that for metal, I was searching for round over bits but only found wood type ones. I may be able to put that in my x2 mini mill just. I can get away with not having the step for the prototype . I guess the best way to get that would be on a 4 axis machine, if anyone thinks they can cnc this if its not going to cost a fortune just drop me a pm

many thanks

Are the radiused edges purely cosmetic, or is sizing critical? You could start with a round bar chosen to give about the right radius on the corners and then machine flats to form the faces? Not sure how you would then handle the stepped-down section; personally I would probably stick the bar in a 4-jaw chuck and turn the corner off on a lathe. CNC isn't the only answer! Be interested to hear how you solve it in the end.

its not 100% critical I'm making another part that this will slide into, I was wondering about getting a 4 jaw chuck for my lathe and doing exactly that but I drew it up and it just didn't look nice at all so left that idea. I had also considered trying to find some 8 sided hex. bar but that doesn't seam to be easily available. I really must get on the case of building a better cnc to do this sort of work although it looks like that will now have to include a 4th axis!

so I purchased the bit but didn't realize er20 collet doesn't go up to 16mm so I had a try on my X2 mini mill however it was a bit of a struggle for it and it didn't turn out perfect, just wondering if anyone in the Sussex area had any sort of machine that would take the bit and could do any of the machining for some beer tokens?

Removing the bulk of material could be done with a TCT wood cutting router bit shaft sizes go up to 12mm, could the transition be finished on a lathe.

Phill

I had a go at machineing the keyway yesterday with my less than perfect cnc designed for cutting polystyrene and although I had to go very slow and I only took 1mm cuts it did get the job done quite well, it would have been even better if I had a long enuff bit too.

Now I just need to find some one with a machine that can do the radius a bit better.

Quote:

---

Originally Posted by phill05

could the transition be finished on a lathe.

---

Only if the design is such that the corner radius is >= half the part width.

-Nick

Quote:

---

Originally Posted by magicniner

Only if the design is such that the corner radius is >= half the part width.

-Nick

---

Which makes it a piece of round bar if its square or not doable if it isnt.

Update: I took the part to a proper machinist and its taken 4 weeks for the guy to put the radius on the corners, I get it back today and my attempt on my x2 mini mill was better! I think 1 out of the 4 sides is ok the rest he has not got the full radius on and one of them is a mile out its hardly touched it! so frustrated I wasted so much time waiting for the guy to do it let alone the £20 I still got charged.
so back to square one! looks like im going to have to try and do it on my cnc but just use a very small step down and then Finnish it by hand.

so the question is whats the best way to machine it like this? running down the length or short vertical passes?

The answer depends on your machining strategy, are you using a corner rounding cutter?
If using an End Mill then I'd go with linear cuts with a square endmill to rough it out to fine steps quickest then vertical passes with a ball end mill to best smooth the corners.

At the size transition step can you get away with a groove around the part? Thus allowing it to fit flush to the step edge but eliminating the machined transition from the rounded corners at the step size transition?

- Nick

Quote:

---

Originally Posted by charlieuk

Update: I took the part to a proper machinist and its taken 4 weeks for the guy to put the radius on the corners, I get it back today and my attempt on my x2 mini mill was better! I think 1 out of the 4 sides is ok the rest he has not got the full radius on and one of them is a mile out its hardly touched it! so frustrated I wasted so much time waiting for the guy to do it let alone the £20 I still got charged.

---

He might have been a Professional Machinist but that just means "does it for money", not that he's any good at it :D
On the bright side he didn't charge enough to spend the time to set it up on a machine, with a down side that it sounds like he didn't :-(

it was a 25x25mm bar and he said he just clamped it in the center so it obviously just defected, and he rotated it around to do each side rather than just clamping it properly and getting it lined up and do one side then just jog it over and do the other. Oh well im hoping I can re use the bit of stock he messed up as at least its not under sized I don't think. All the more reason to build a better machine myself.

I cant use the corner cutter I got as it will not fit in er20 collets so going to have to use a straight and a ball nose.
I don't quite understand the last bit your saying but the part has to fit down a tube with a fairly tight tolerance.

many thanks

Do you actually need the round profile?
Would just cutting the corner off with a square endmill to create clearance work?

Quote:

---

Originally Posted by charlieuk

I don't quite understand the last bit your saying but the part has to fit down a tube with a fairly tight tolerance.

---

What's the step for?
Does the smaller section fit into something?
Does the step provide location?

Charlie, I did read this a while ago and do have some comments.

Firstly is understanding the problems created by the drawing/design. Cad means you can draw anything these days but that doesn't mean you can make it easily if at all in some cases, also vs cost of the designed part as apposed to a re-design that will do the same thing but is far cheaper/easier to produce. These are wise words worth heeding to anyone who is a little green. Get advice from someone who actually knows what they are doing, who ever it is.

It's a big problem for guys like me in the trade where we constantly get drawings from people who are not trained/ brought up in the trade this also includes so called professionals at times. Someone taught them how to use cad at some point (including universities and colleges) with no understanding of manufacturing The only proper transition is from the shop floor to design, often with only a few exceptions these days. This is the only way people learn how to design properly. This is becoming a huge, huge problem for people like me now and it is all but costing me my living by having to advise and sort designers lack of knowledge/ability unpaid, consuming hours of my time every week. Understanding the cause of the problem helps you find a solution for the future.

Sadly this will never be addressed properly in the Uk unless we go back to being a proper manufacturing nation using old school methods of learning.

Understanding the above comments would have helped you with your part.

The small square shoulder at one end of the part is the problem as you now know from others. So you have to design around that problem. Is it doable as it is.... hmmm yes probably but it makes life difficult and expensive, so look for an easier solution, put a rad where that square shoulder is so its a transition from one square to the next, this will allow you to 3D the rad and gets rid of the square corner problem. You would have to use a small ball nose (explained later) lets say 6mm so put a 3.5 rad in that corner so there is no collision of cutter rad to part rad. If that square corner is used as a stop then put a small pin in place of the stop, it will do the same thing but far cheaper and easier.

The other very obvious solution is the turn the part on its end and machine in that orientation the square corner then becomes a non problem its a simple 2d path on a cnc. Not having dimensions I have no idea how long that step is or if its to long to do in that orientation. Information is power provide people with more info then they are better equipped to help you.

The rad on the edges is something that needs to be considered, (assuming rad cutter is out of the equation due to size and cost) because it's 25 mm square with 8 mm rads, that means in real terms when you come to do the last set of rads you have 25-8-8 which leaves 9mm of flat left to hold on, this is fine for the first 2 rads but lets say we are going to use a 6mm ball nose for finishing. The cutter will be at the furthest point from the ball at the lowest part of the rad being machined this then leaves 9mm-6mm this gives you 3mm to hold on plus you need some clearance for the cutter so 2 mm to hold on... not a lot! This is based on a machinist who would naturally look at a vice/vices as the cheapest and easiest option to hold the part.. a smaller ball nose will give you more clearance but you sacrifice rigidity and of course more risk of breakage with smaller cutters. The obvious solution is 2 tapped holes in the part either end and a plate with 2 back stops (dowels) to clamp the part to, either leave the job long and clamp on the ends and cut that off later and machine, or two tapped holes to clamp through the plate or a variation on that theme. This method leaves you with 9mm + 8mm = 17mm of free space for the ball nose to do its job. Tons! Plus you can now use a bigger ball nose for better cutting and more rigidity.

Lastly, the machining process you have used is wrong. With this part you would:

1] Do the rads first.
2) Holes through the V (in a vice for ease)
3) Only then would you do the v cut out (in a vice) with the part being machined supported in the vice and not extended out from the jaws.

The reasons are as soon as you cut out that V you take away support and rigidity from the part to do the rads this means deflection caused by the V having the material machined away, This is about good standard machine shop practices and getting into good habits and understanding the processes a machine shop guy should employ.

Yes you would natural machine the rads along its x axis (omitting the step as it is) from left to right or right to left with the z and y stepping progressively is your software will allow this machining strategy. Rough first then finish with either a ball or bull nose. A bull nose would help would help with the clearance issues if trying to hold the part in a vice to produce the rad

Regarding the guy that did the work. Sorry if you managed to find one of the non competent ones out there, some of the issues i raised may well be why you have not had a complete job returned, but the bottom line is, he charged you nothing and if you pay peanuts.... well sorry to say you got monkeys. What he charged you would cost me more to keep the doors of my works open for the time the job would take.. ie I would lose money.

We have dealt with each other before charlie as you know and nothing is said with malice I'm just being straight, nothing personal.


All the best.

I have done a way with the step now to simplify it so its just the 8mm radius I'm stuck on which I cant really get rid off. It slots into something on one end and something else slide over it and is located in the center.
I have been trying to figure the cam out on fusion360 but haven't found the right strategy yet. if anyone who uses fusion has any tips it would be great.

A quick look suggests to me that Adaptive Clearance with Contour Finishing might get you where you want to be, Autodesk documentation isn't the greatest though and I'm a BOB-CAM user.
Regards,
Nick

I'm with M_c (post #19) on this.

Clamp the bar in a V-Block held in the vice and mill each corner off the square one edge at a time (fliping/inexing the bar over in the V-Block for each edge and only mill as far as the step needs to be), to in effect give you the octagonal shape you first thought of, where it goes into the other tube.
Set an end stop for the bar to butt up to and use the end of the cutter not the side.

There's other methods, but this is the quickest (if youve got a big enough V-Block) and easiest with limited equipment.

Nick.

cheers I think I have managed to get a tool path sorted so will give it a test tomorow