I am desiging a part that needs to have a volume milled out (~7.8" long, ~5.5" wide , and ~3.4" deep). I am assuming that a 1" diameter end mill will be used and the material is 7075. Is this a reasonable depth to mill out? Will I need to look for a shop with special tooling?
Thanks in advance for your help/comments.
The optimum is a depth of 2 times diameter = which means a cutter configuration of 1. dia 2. deep, .5 dia 1. deep .25 dia .5 deep etc
Aerospace 3 to 1 which is a std (for corner radius reasons) works ok but is not as fast
4 or deeper works when carbide ext type tools are used but the depth of cut is less and the max ext length is a matter of maching rigidity (not to exceed maybe 10in from the gauge line of a 40 taper, 14 from a 50 taper)
Since the part you are discribing is a hog out you may want to send quotes to shops having Surfcam, they have a technology that handles the deeper depths of cut much better than conventional style tool paths.
hope this helps
na, havent messed with 7075 in years but id guess, 900 sfm with inserts, (2" 5fl ) im gonna throw out a gut instinct of 4 min each , 1.5 DR then 2" 5fl insert then a fininsh end mill type thingy
drill -.02 min max
rough- 2 min +tool change
fin - 1 min
so like if u want production. 4 min each including load/ unload,
can i have a cookie now?
special tool shop. na, anyone can do, cost, volume and availability is what you need to look at
Piece of cake...Really, it's not the easiest cut in the world but I've seen much worse. You shouldn't have a problem finding someone to make it. If you do, then there are a lot of really, really busy machine shops out there that don't need the work.
what do the corners look like as this could be the bigest problem (i.e., .125 radi would make for a fun time. The rest would be done as plung mill ad the finish passon floor and walls. Oh whats the wall thickness as this adds to the fun.
can you tell me why they would have better technology, what tooling/machines they have that an ordinary production shop wouldn't have.Originally Posted by camaru
I agree with 'justcncit'. You don't "need" Surfcam to do this. The part in question (based upon the reference dimension) isn't that tough. Many CAD systems (if not all) can accomodate to this. 3.4" deep isn't that tough. Do it all day long. As Verfur said, your corner radius and maybe any other internal features will add to the complexity. The tools required from what we know of the part is nothing special...
It's just a part..... cutter still goes round and round....
Not to ask a dumb question, but when you say "diameter times 2", are saying that you do this depth in a single action?
I'm still trying to figure this stuff out and I've never tried cutting anything even close to that deep in one shot...maybe .1 inch with a 1/2 carbide.
Chris64,
No not in one pass, rather it would be the maximum reach of the standard length tool. After that, then you have to opt for something longer, and the extra reach means a greater risk of chatter. So then the depth of cut per pass has to generally be decreased from what was suitable for the standard length tool.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thanks and that's why I asked...I thought it sounded odd but you never know what better quality machines are capable of.
So what are the approx depths people usually cut? I've found in most cases to go .02" on both steel and alum for safety sakes. I'm just taking babysteps with it but I think I should probably going deeper especially on alum (6061T6).
There is wide range of opinion on depth of cut. There are many many variables such as tool material, work material, clamping method, coolant availability, the grind style of the tool, tool coatings, toolholder grip style, etc.
The ultimate restriction would be machine horsepower: the 'unit horsepower' factor gives one an idea of how many cubic inches of material can be removed per minute ,per horsepower available. This is not necessarily 'motor horsepower' in this day and age of VFD drives, where a motor running at half of its nameplate rpm is only running at 1/2 its nameplate horsepower. So that can make it seem like a machine poops out before it should, however, the restriction is necessary to prevent overheating of the motor under continuous duty conditions.
So unit horsepower is the ultimate restriction. Cutter loading could be considered as the first or second ultimate restriction. If it cannot throw the chips out, it will break off.
Roughing endmills can often rough at a depth of cut equal to the cutter diameter, so I've heard.
Finishing endmills can rough at a depth of cut equal to the cutter radius. This would be under full width of cut conditions.
For lighter finishing cuts, the whole length of the flute is fair game so far as depth of cut is concerned.
Using inserted carbide endmills, I've had better success using them for full width roughing in steels in the range of 0 to 1/4d as depth of cut, and cranking the feedrate up high to compensate for lower depth. This method seems to give a more natural edge wear life, particularly on the corner of the insert. The insert wears out and gives ample warning of its wear condition by throwing sparks. When running an insert cutter at deeper cuts, the edge failure tends to be more catastrophic, and sudden, and the supporting corner of the steel body of the tool usually is spoiled when the insert fails catastrophically.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Posting Permissions
LinkBack URL
About LinkBacks
