I am not sure if this is possible, but I am attempting to design this part with 0.125" radius inside total depth of 60mm. It is aluminum. I ran a check in solidworks and it mentions a depth error. Without EDM is there a way to cnc this part. The center wall is 1.5mm thick also. The part is 1" x 2.5" x 2.4" depth. The holes would go right through the part. Is this possible
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
How deep can you cnc 2
- Thread starter valmeidan
- Start date
I assume you're talking about the 4 corner radii in each pocket. You've got a .25" diameter end mill that would need to be about 2.5" long. That's a 10:1 ratio on the end mill. That's pretty tough even with carbide. You might want an experienced machinist to take a look.
- Thread starter
- #3
If you had more wall thickness then I might suggest some kind of corner relief, but with your wall thickness I'm not sure if it buys you much.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
MartinShane
Mechanical
If the pocket passes all the way through the part I would think that it could be approached by milling half the depth from each side, but 1) I'm no machinist, and 2) that would introduce its own set of problems (costs) etc.
Alternatives are probably numerous and depend on what your application, dimensional tolerances, and production volume will allow. More information about how the part would be used and how many would be made would probably help get better suggestions.
Alternatives are probably numerous and depend on what your application, dimensional tolerances, and production volume will allow. More information about how the part would be used and how many would be made would probably help get better suggestions.
Quickest solution would be to figure out your maximum inside radii? If you could live with a .25" radius or larger, things will be better. If machined from both ends, what amount of offset can your requirement allow? Are the holes just for lightening?
"Art without engineering is dreaming; Engineering without art is calculating."
Have you read faq731-376 to make the best use of these Forums?
"Art without engineering is dreaming; Engineering without art is calculating."
Have you read faq731-376 to make the best use of these Forums?
ornerynorsk
Industrial
Not practical depending on your finish and tolerance requirements. Sinker EDM might be something to consider. No allowable taper on the inside sidewalls?
How high of volume part is this? Impact extrusion may be worth checking into, as well as diecasting.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
How high of volume part is this? Impact extrusion may be worth checking into, as well as diecasting.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
If this is from billet the corners can be drilled out then the pocket would be milled. In my opinion it is machinable, but not ideal or easy to achieve a good finish. It will depend somewhat on your machinist producing the part, when in doubt I would defer to their recommendations.
Comprehension is not understanding. Understanding is not wisdom. And it is wisdom that gives us the ability to apply what we know, to our real world situations
Comprehension is not understanding. Understanding is not wisdom. And it is wisdom that gives us the ability to apply what we know, to our real world situations
-
1
- #9
ornerynorsk
Industrial
Wait a minute, just re-read the OP. The holes go through. Wire edm on low volume, conventional extrusion on medium/high volume.
Even drilling the corners, you're going to get a lot of chatter from a depth like that trying to mill it.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
Even drilling the corners, you're going to get a lot of chatter from a depth like that trying to mill it.
It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.
-
1
- #11
valmeidan,
Does the part have to be done by CNC?
The corners may be doable with a broach.
The ultra deep radii may be doable by using a very slow feed, making the part much more expensive than it would be with more reasonable dimensions. Maybe this is acceptable to you.
If your radius is .125", the CNC people will not use a Ø.250" cutter. They will use something smaller, so that they can feed all the way through the radius.
Have you talked to a machine shop yet. If they come back and say they can do it, somehow, you should be fine!
--
JHG
Does the part have to be done by CNC?
The corners may be doable with a broach.
The ultra deep radii may be doable by using a very slow feed, making the part much more expensive than it would be with more reasonable dimensions. Maybe this is acceptable to you.
If your radius is .125", the CNC people will not use a Ø.250" cutter. They will use something smaller, so that they can feed all the way through the radius.
Have you talked to a machine shop yet. If they come back and say they can do it, somehow, you should be fine!
--
JHG
CorBlimeyLimey
Mechanical
If single piece or low volume, wire EDM is definitely the way to go. It's relatively fast, accurate & cheap and you may even be able to use the cut-out pieces for other parts.
If CNC is an absolute must, hog out with a larger bit, and then carefully plunge cut the corners from both ends with a Ø1/4 slot drill. Clean up the run-outs with same or end mill.
If CNC is an absolute must, hog out with a larger bit, and then carefully plunge cut the corners from both ends with a Ø1/4 slot drill. Clean up the run-outs with same or end mill.
racookpe1978
Nuclear
Do the 4x holes in the corners with a 3/16 or larger (maybe 7/32 or 0.200 inch for example) dia ball-end plunge mill/drill. those will get you 4x square "corners" to the right depth withe ach corner at the right lace, but with rounded ends
It's only 60 mm - just over 2 in deep "pockets" - so do the pocket next. Flat bottom, to the right depth. You have room now, so use a shorter end mill that's fairly rigid: may a 1/2 inch dia. Go the the exact depth across the floor.
Change tools to a finishing 1/4 inch dia ball end mill; but "aim" the tool so it is angled down and into the 4x corners at a 45 degree down angle, 45 degree sideways angle. Trim the 4x corners with the 0.250 ball bit so you are cutting from the top down cutting a radius in the radius in the corners with a rigid tool.
It's only 60 mm - just over 2 in deep "pockets" - so do the pocket next. Flat bottom, to the right depth. You have room now, so use a shorter end mill that's fairly rigid: may a 1/2 inch dia. Go the the exact depth across the floor.
Change tools to a finishing 1/4 inch dia ball end mill; but "aim" the tool so it is angled down and into the 4x corners at a 45 degree down angle, 45 degree sideways angle. Trim the 4x corners with the 0.250 ball bit so you are cutting from the top down cutting a radius in the radius in the corners with a rigid tool.
powerhound
Mechanical
This part just doesn't look very difficult. Give it to a machine shop and they'll quote it. I'd be more concerned with the chatter on that thin wall than the corners but that's not an insurmountable problem. Unless you have some rigid requirement that you haven't mentioned, it won't be an issue. The larger you can make the corner radius, the better but a .125 isn't that big of a deal over that depth.
John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
MikeHalloran
Mechanical
The only problem with drilling the pocket corners first is that you need a really fast spindle to make a nice hole in aluminum. ... up to 18,000 rpm would be nice.
If I had only ~6,000 rpm available, I might hog out the pocket with big indexable 2flute drills of a diameter nearly the smaller pocket side dimension, then broach the remainder of the pocket and the corners.
OR just let the CNC owner decide how to make the moderately deep through pockets with moderately difficult corner radii. There are a near infinite number of ways to do it with canned cycles, and shortest cut time may not be optimal for cost, considering cutter and machine availability, chip removal, presence or absence of an attendant, etc.
I.e., just send it out for quotes, with a full set of dimensions and tolerances please, and see what you get back.
Mike Halloran
Pembroke Pines, FL, USA
If I had only ~6,000 rpm available, I might hog out the pocket with big indexable 2flute drills of a diameter nearly the smaller pocket side dimension, then broach the remainder of the pocket and the corners.
OR just let the CNC owner decide how to make the moderately deep through pockets with moderately difficult corner radii. There are a near infinite number of ways to do it with canned cycles, and shortest cut time may not be optimal for cost, considering cutter and machine availability, chip removal, presence or absence of an attendant, etc.
I.e., just send it out for quotes, with a full set of dimensions and tolerances please, and see what you get back.
Mike Halloran
Pembroke Pines, FL, USA
I'll throw another option in on top the other excellent suggestions:
If the internal finish is important and you need the 60mm pocket depth then another option would be to split the part in two (or 3) and then vacuum braze them together.
Wave guides are made this way sometimes.
The 60mm depth requirement is somewhat confusing if the holes go all the way through...if you could post another picture showing that detail it might help everyone understand your requirement better.
TobyK
If the internal finish is important and you need the 60mm pocket depth then another option would be to split the part in two (or 3) and then vacuum braze them together.
Wave guides are made this way sometimes.
The 60mm depth requirement is somewhat confusing if the holes go all the way through...if you could post another picture showing that detail it might help everyone understand your requirement better.
TobyK
MikeHalloran
Mechanical
The reason SW declared a depth error is that the OP built the cavities as if they were blind. SW interpreted the breakthrough as an unintended consequence. There are simpler ways to make a through hole in SW, that will not confuse it.
Mike Halloran
Pembroke Pines, FL, USA
Mike Halloran
Pembroke Pines, FL, USA
Another way to make the part, even with sharp internal corners and blind pockets, would be DMLS. DMLS is a bit pricey and would only be practical for small quantities, but the process gives good dimensional accuracy and can produce monolithic parts with geometries that would be difficult to make using conventional machining. Any DMLS machine can easily handle a part of this size. Also, DMLS normally doesn't require tooling, which saves some cost versus other processes such as sinker EDM or broaching/shaping.
Regards,
Terry
Regards,
Terry
- Status
Similar threads
- Question
- Question
- Locked
- Question