[alexccmeister]

Hi All,

I had these parts milled by a company. As the cost is high when someone is doing it. I thought I will do it myself. So currently in the process of getting myself a cnc mill.

I have a few questions as to how some of the parts are milled? If you look at the photos, circled red are the recess and protruding parts that I am curious as to how they actually milled it. Its 90 degrees so I don't see how they can use an endmill to mill it without having some curve chamfers. Can anyone advised?




Thanks in advance.

[turmite]

Broach or edm and I don't think you can broach a blind hole. I am not a machinist but have been around a lot of it. You have your work cut out making these with just one machine. I'd be willing to wager that the price you paid for them will not look nearly so high when you get through with the process of making them yourself! Ask me how I know!!!!(nuts)


Mike

[alexccmeister]

Broach or edm and I don't think you can broach a blind hole. I am not a machinist but have been around a lot of it. You have your work cut out making these with just one machine. I'd be willing to wager that the price you paid for them will not look nearly so high when you get through with the process of making them yourself! Ask me how I know!!!!(nuts)


Mike

Hi Mike, Thanks for the quick response. I know its not going to be easy to do this after reading some of the threads here. When you say the part may need to be milled with a few machines, what are the other machineries that the fabricator may have used to do this?

I might not be bothered to mill this out eventually and let the expert do it but knowing how its done would really help me to understand more about milling.

Its so funny that the fabricator informed me before fabricating the part that they couldn't do a perfect rectangular hole for me as shown in the model. So what they ended up doing was giving me a rectangular hole with curve chamfer on all four corners. Now I know how they made that. By using an endmill right? So if they can't do a perfect rectangle or square, how come they could do a perfect 90 degree recess and a protrusion?

I will probably ask them personally but if anyone can offer me an answer here. that will be great. I doubt very much if they would want to tell me so mcuh info on this seeing its their business.

Here is the picture I mentioned about the square hole.



They ended up giving me this instead.



Thanks

[JerryFlyGuy]

So your building a cnc mill to make this part? I'd think you should have looked at EDM, I don't think you'll find that you can make these on a mill, that is unless they are huge, and you have a teeny 5 axis head to reach inside there and cut them. 90deg corners on a milled part like that is pretty much outta the question..

Jerry

[matsuura]

They probably did this in many pieces and then welded them.

[DareBee]

Mill then EDM

[turmite]

Hi Mike, Thanks for the quick response. I know its not going to be easy to do this after reading some of the threads here. When you say the part may need to be milled with a few machines, what are the other machineries that the fabricator may have used to do this?

I might not be bothered to mill this out eventually and let the expert do it but knowing how its done would really help me to understand more about milling.

Its so funny that the fabricator informed me before fabricating the part that they couldn't do a perfect rectangular hole for me as shown in the model. So what they ended up doing was giving me a rectangular hole with curve chamfer on all four corners. Now I know how they made that. By using an endmill right? So if they can't do a perfect rectangle or square, how come they could do a perfect 90 degree recess and a protrusion?

I will probably ask them personally but if anyone can offer me an answer here. that will be great. I doubt very much if they would want to tell me so mcuh info on this seeing its their business.

Thanks

I forgot to ask and made an assumption that this was metal. Is it metal or plastic? If plastic it would be injection molded, but the additional machines would still be needed.

If the "square" hole had radiused corners it was milled. I would approach it by lathe and edm, for the part and a mill to make the electrode for the edm, so there is three machines.


Now where is HU when you need him?

Mike

[precisiontork]

This part could be made on a mazak integrex and you could do internal hobbing or broaching to make internal parts but this is a expensive machine around 300,000.00 for a small one

[alexccmeister]

Hi All,

Thanks for all your replies. The part is aluminium and the internal diameter is 70mm exactly. The thickness of the wall is 3mm. Well, the person informed me that the whole thing will be milled. She didn't mentioned anything about any other type of machine to do the job.

So your building a cnc mill to make this part? I'd think you should have looked at EDM, I don't think you'll find that you can make these on a mill, that is unless they are huge, and you have a teeny 5 axis head to reach inside there and cut them. 90deg corners on a milled part like that is pretty much outta the question..

I would love to do this with a CNC machine of my own, but if its too difficult, I may need to redesign the parts taking account of the limitation of the cnc mill. Can a six axis machine do this part? I am sure their equipment is expensive, but unless their chuck or what evre is holding the endmill is small enough to get into a 70mm round space, I dont see how they can do it. I think EDM method may be the answer.

If the "square" hole had radiused corners it was milled. I would approach it by lathe and edm, for the part and a mill to make the electrode for the edm, so there is three machines.

I am pretty sure this is milled as well. But that begs the question why they didn't do EDM on this part when they could do it on the most difficult part. I don't get it. They specifically told me they can't do it when I ask if they can give me sharp corners. Not that they won't do it as the square corner isn't that critical and I can live with round corners. They just can't.

They probably did this in many pieces and then welded them.

I am not so sure as the part is really smooth and nicely done, no indication of any welded joints. I am convinced it is milled from a solid block of aluminium.

Thanks guys. I will put in an email to the fabricator and see if they can offer an answer. If they do, I will post the answer here. Thanks.

[fyffe555]

Interesting looking part - what does it do?

I have to ask; Does the function of the part *need* the difficult to machine elements as designed? Could you make the part easier to machine by including radius to allow simple milling?

Too often a part gets designed by people without much machine room experience and the part is unnecessarily hard or expensive to produce...

[holbieone]

to make this part you will need to

mill ,broach and or scrape

or cast then finish with machining process

or forged then finish with machining process

or precision cast to finish

[alexccmeister]

I have just emailed the fabricator regarding this issue. Will see what they have to say.

Interesting looking part - what does it do?

I have to ask; Does the function of the part *need* the difficult to machine elements as designed? Could you make the part easier to machine by including radius to allow simple milling?

Too often a part gets designed by people without much machine room experience and the part is unnecessarily hard or expensive to produce...
Reply With Quote

Its part of an imaging device I am working on. The prototype is already done by the fabricator. real; professional. Cost me a bomb having it made by a third party. So planning on getting some of the parts done myself. Here's the part after it was made, polished and anodised.



I could probably just have the mill cut the piece out but with the curve chamfer instead of a 90 degree corner. Probably a very small end mill will do the job to finish off the corner portion?

[nupeswv]

The removal of material in the blind hole can be done by broaching using a single tooth custom broaching tool...I have done similar jobs in aluminum by mounting the part in a lathe chuck, locking the chuck solid with a brake/wedge/strap. The tool is mounted on the tool post and centered in the part using shims, and the cross slide is used to for depth of cut, the carriage is used by hand as the ram for broach. Set up a stop on the carriage just shy of the end a few thou so the chip dont break the tool. You can hand grind the tool out of square tool steel blank starting with a minimal relief angle. ...couple degrees...if u get chatter of deflection increase it a bit till its right. If you use too much it will dig in much like a chisel. Use WD 40. The part that extends into the ID can be done by machining and the broach can also be used to square up the radius thats left. I am not sure what the accuracy needed is...the tool can be made to size, or the chuck can be indexed a bit on an undersize tool with a small sacrifice of angle on the edge. Hope this helps.

Emmery

"Quit complainin, I wanna see chips'

[alexccmeister]

Hi Guys,

Got the reply from the fabricator,

Dear Alex,

Nice to hear from you.

CNC is unable to achieve 90 degrees angle as the cutter are all round. So there will definitely be radius and the degree of radius depends on the cutter that is used. For Pic 1, the circled area had actually been manually polished after machining. Slight polishing was done to ensure there is no problem with fitting. This is why the corners appeared to be 90 degrees. For the rectangular hole in Pic 3, no polishing was done. Hence, the raw radius is more visible.

Hope the above clarifies

Looks like they used the broach method of getting rid of the chamfer. A really good job I must admit but I guess i can cut cost by not doing it this way. Will redesign the part so it can be easily milled.

[alexccmeister]

The removal of material in the blind hole can be done by broaching using a single tooth custom broaching tool...I have done similar jobs in aluminum by mounting the part in a lathe chuck, locking the chuck solid with a brake/wedge/strap. The tool is mounted on the tool post and centered in the part using shims, and the cross slide is used to for depth of cut, the carriage is used by hand as the ram for broach. Set up a stop on the carriage just shy of the end a few thou so the chip dont break the tool. You can hand grind the tool out of square tool steel blank starting with a minimal relief angle. ...couple degrees...if u get chatter of deflection increase it a bit till its right. If you use too much it will dig in much like a chisel. Use WD 40. The part that extends into the ID can be done by machining and the broach can also be used to square up the radius thats left. I am not sure what the accuracy needed is...the tool can be made to size, or the chuck can be indexed a bit on an undersize tool with a small sacrifice of angle on the edge. Hope this helps.

Emmery

"Quit complainin, I wanna see chips'

HI Emmery,

Thanks for the method of fabricating. Looks like the same method was used. So at least I know they didn't use a 300k machine to do the job. Just your everyday hand filing works.

[Mcgyver]

The removal of material in the blind hole can be done by broaching using a single tooth custom broaching tool...I have done similar jobs in aluminum by mounting the part in a lathe chuck, locking the chuck solid with a brake/wedge/strap. '

I've done the same, but in a blind hole? standard practice with a shaper would be to drill a hole at the end of the flat so the tool doesn't slam into the shoulder with no place to go. broaching in the lathe or mill is similar challenge if its blind. then again the old timers would have just had at it with a chisel and hammer, so a lot is possible with simple tools.

Alex i think you've come to the right conclusion, redesign the part. This is why its so valuable that designers also understand machining and imo where disdain between machinists and engineers comes from.

whats a bomb btw? its all relative, but its a big assumption that you can bring it in house and save money. If the outsourced supplier was selected in a competitive environment, and his price is based on the cost of his equipment, tooling and time, you are going to incur the same costs or more given you may not be as efficient as the specialist.

for production, would plastic work? i don't know loads or tolerances but the part could easily be injection molded.

[alexccmeister]

Hi Mcgyver,

Your suggestion is a lot work me and I will probably not see myself slaving away filing and polishing the parts after being CNCed. So redesign it is.

"bomb" is just a figure of speech I use when something is expensive. I haven't decided what I will do as far as the part fabrication are concern. But once my cnc mill is here and all set up, i will be doing some fabrication myself to see how much I can do. It probably won't be as good as the expert, but if I don't try I wouldn't know. As there are many parts that I need to fabricate out of both plastic and metal, I may just do some of the simple parts and leave the rest to the expert and cut cost there.

The other reason why I would want to do it myself is that the parts I am doing are in the early stage of the design and the one that was made by the expert was a prototype. Still need some more testing before I finalise the design. So the parts I need made are costly and although not as costly as a new set of cnc mill, I will be spending quite a bit having them made and they won't necessary work. So its back to the drawing board redesigning and going back to the expert . Very troublesome, so why not get a cnc mill and I can test all i like until i get it right. I gain experience and a set of cnc mills. Oh! and the nearest cnc milling company to me is by a plane ride that takes 2 hours to get there. So that too was a deciding factor for me to go with my own CNC mill.

I have thought about plastic injection molding. But I can't source for the right equipment where I live and most of the parts are in aluminium anyway.

Thanks.

[nupeswv]

I did not have a problem doing blind hole in aluminum with broach but solved the problem on a steel part by using a small woodruff cutter to cut a 1/8 " wide crescent shaped relief at the end of the groove. The tool and chip can run out there without worry of breaking tool. It also does not show as a hole on the exterior of the part if cosmetics are a concern. The job can be simplified also by running the woodruff cutter down the groove to remove most of the material to proper depth, mark with magic marker and use the broach tool to just clean up the rads in the edges till mark is gone. The cutter needs to be of the offset side cutting variety.

[lerman]

In doing your re-design consider:
which aspects of the design are functional
which parts of the design are esthetic
which parts of the part are visible

An example: I had a part that had a rectangular LED display passing through the aluminum housing. Since the corners of the LED had a small radius, it was not cost effective to cut a rectangular hole. Instead, I made a hole with 'dog ears'. I let the cutter run past the corner by an amount equal to the radius and then back up before doing the adjacent side. Since there was an overlay covering the hole, the end user couldn't see the funny looking hole and I could just mill it without any secondary operations.

Keep us informed as you go through the redesign. I'd be interested in seeing the next few iterations.

As a reference, I went through at least ten different designs on the manifold of the anesthesia machine we sell. And that doesn't count the designs that were just on paper.

Ken

[notallhere]

Looks like a milled casting.