What's new
What's new
By:
Advanced search…

reaming, 3 pass vs 4 pass

G

god_paul

Aluminum
Joined
Dec 11, 2013
Location
MI
in pic, you can see the interrupted gap that the semi-finish and finish reamer has to come through

the upper pic represents a cast body
the lower pic represents finished part

here are 2 proposal:
proposal A
1. use drill to drill through the bottom cap
2. use drill to enlarge the entry hole so that the roundness/position of the entry holes will be nice for the next reaming process
3. use semi-finish reamer to go through all features
4. use finish reamer to finish the features

proposal B:
1. use drill to enlarge the entry hole so that the roundness/position of the entry holes will be nice for the next reaming process
2. use a CENTER cutting semi-reamer to go through all features, INCLUDING the bottom cap
3. use finish reamer to finish the freatures


P.S
drill is made by carbide
semi-finish and finish reamer are PCD reamers...

which one will you choose?
does this depends on feature length?

thank you
Capture.JPG
 
You didn't say what the part does, or what material it is, but in any case the more steps the less the following reamers will run out and the straighter the finished hole will be. However, if this casting is some kind of valve, with a spool that has to seal in that bore, I don't think reaming is going to give you adequate finish or cylindricity. Count on leaving .001 and honing it.
 
hi Oldwrench, sorry, forgot this

the material is cast aluminum
and you are right it is spool and the vale will slide through those gap

but does honing will take more time?
 
I'd start with a G-land (or 4-land) PCD tipped drill. This type of drill has 2 flutes and 2 guiding lands. The guides help to assure a good straight hole. As long as the reamer is guide padded, roundness shouldn't be an issue.
 
sfriedberg said:
Yes, but you don't have a choice. Reaming will not give a functionally satisfactory surface.
Click to expand...

hi sfriedberg

in our production, we dont use honing process.

i ask today and check the surface finish, they are all mirror like surface

is this trustworthy?
 
What are the specifications for the hole?

Roundness and Straightness
Concentricity (if specified)
Or
Cylindricity
Diameter tolerance
Location tolerance
Surface finish + tolerance

I'm just going to guess on some of these..... lets see how close I get...

I say 0.004 mm on roundness
+/- 0.007 mm on diameter
Straightness of 0.008 mm over length of bore

How close am I?
 
Tonytn36 said:
What are the specifications for the hole?

Roundness and Straightness
Concentricity (if specified)
Or
Cylindricity
Diameter tolerance
Location tolerance
Surface finish + tolerance

I'm just going to guess on some of these..... lets see how close I get...

I say 0.004 mm on roundness
+/- 0.007 mm on diameter
Straightness of 0.008 mm over length of bore

How close am I?
Click to expand...

sorry for the late reply....

fro roundness, it's not specified on the print...
for concentrictiy, 0.007 mm
diameter: +/- 0.011 mm
location: 0.5 mm
surface finish: 1.25 um
 
by the way,
Tonytn36

for finish reamer, do you recommend straight flute or helical flute, what's your supporting evidence?
 
god_paul said:
by the way,
Tonytn36

for finish reamer, do you recommend straight flute or helical flute, what's your supporting evidence?
Click to expand...

No finish reamer.... finish padded boring bar.

What I'm suggesting to try......(No guarantees, but I've done this and it works on interrupted bores)

G-land PCD tipped drill to make the hole Ø0.5-0.75 mm undersize.
Then a padded, inserted PCD boring bar for finish. It will probably have 2°-5° of axial rake and be single cutting edge. (If I can get time tomorrow, I'll grab a picture of one.)
DONE

As I mentioned above, I did quite a bit of testing on this set-up. It worked well, but didn't suit several other constraints of our manufacturing system.

Call the Mapal guys, show em what you got. They will offer a solution that works. (May take forever + 10 days to get it if they don't send it to SC plant to get it made, but it will work.)
 
Tonytn36 said:
No finish reamer.... finish padded boring bar.

What I'm suggesting to try......(No guarantees, but I've done this and it works on interrupted bores)

G-land PCD tipped drill to make the hole Ø0.5-0.75 mm undersize.
Then a padded, inserted PCD boring bar for finish. It will probably have 2°-5° of axial rake and be single cutting edge. (If I can get time tomorrow, I'll grab a picture of one.)
DONE

As I mentioned above, I did quite a bit of testing on this set-up. It worked well, but didn't suit several other constraints of our manufacturing system.

Call the Mapal guys, show em what you got. They will offer a solution that works. (May take forever + 10 days to get it if they don't send it to SC plant to get it made, but it will work.)
Click to expand...

hi Tonytn36,

based on your feedback, i got several questions
1. our PCD reamer is brazed PCD reamers by UM, so your inserted PCD reamer(boring bar) is recommended by Mapal or you have history of using this design? any advantage of inserted PCD reamer VS. brazed PCD reamer?

2. how often do you change tool (does it give you trouble in setup, or some weird broken/chipped problem?

thank you :)
 
Ok... I'd like you to drill the piece and then use a half round drill instead of reamers. The half round drill can not go oversize, and it's stiff enough to bridge the gaps. I'd first try it at around 1000 - 1500 rpm, chip load 1% of the hole diameter and work your way up. I say this because they don't chatter.

Regards,
Stan-
 
Tony,

How do you deburr a feature like this? We tried a lot of things, including a waterjet. It's still the worst part.
 
ewlsey said:
Tony,

How do you deburr a feature like this? We tried a lot of things, including a waterjet. It's still the worst part.
Click to expand...

I'd check out abrasive brushes, a bunch of companies make them. From Osborn:

ATB Products - Osborn [scroll down for "Internal Finishing Brushes"]

They can tailor abrasive grain size, filament OD, density, twist, etc. to product a one-pass deburring tool that can be added to the inline process.
 
Milland said:
I'd check out abrasive brushes
Click to expand...

Been there. I don't know of one that can reach all the way into a bore like this and do any good without rubbing the shank on the bore. Also, they wear quickly.

We tried a cascade machine, but it messed with the surface finish of the faces.
 
Well, ideally the guy who designed the casting put cast-in transitions that prevent a burr. That does require a more expensive mold however. About the only way I see to deburr that thing is either a brush as mentioned above, or a burr tool that is circular interpolated in each cavity. For high volume, it would certainly pay to go the more expensive mold route.

There is also the gas-fired option (burning them off) but not sure if that would work with the geometry of a feature like that, nor what that may do distortion-wise to the part.
 
You must log in or register to reply here.

Similar threads

J
Concentric Drilling/Reaming
Replies
15
Views
419
wesg
W
N
Brass bushing ID reaming/boring
Replies
7
Views
317
john.k
J
O
Plunging into 17-4 H900 with a micro tool
Replies
7
Views
442
OliviaB
O
F
What is the most efficient way to cut a counterbore?
Replies
19
Views
1K
Garwood
G
H
Brass Mouthpiece Backbore - Reamer vs....?
Replies
10
Views
987
harrison.t.reed
H








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top