A few machining theory questions.

BRIAN.T · Jan 9, 2019

I've been pondering a few things lately, so I'll ask you guys.

Question one, with all things equal, do you guys step down or step over. Now obviously most of the time there is an obvious logic behind one or the other. But certainly there are other times when either one would do. I personally find myself stepping over. Is there a definitive reason to gravitate towards one of the other.

Second, again variables aside, in a situation where your material removal rate is equal, either by high speed, low stepover or low feed high stepover, which would be less aggressive on the part. Obviously high speed is better for the tool, chip thinning and all, but which is better on the part. Say to keep a part from pulling out of a vise. Im not sure. Any ideas?

Discuss!

Hazzert · Jan 9, 2019

I prefer to go as deep as possible to spread the wear over as much tool that I paid for. If a feature is 1/2 D or less then I will normally just run a regular pocketing routine with a 60 or 70% stepover.

For a work hardening material a wider slow cut may be better to stay ahead of the work hardened skin and I would think that the less entries and exits through that the better. Now that’s not to say I’d bury the cutter and grind out pockets but maybe a 8% stepover instead of a 5 or 6%.

When it comes to pulling out of a vice a higher helix angle will have less axial lift and would be a better choice. An indexable might be an even better choice with almost no helix.

BRIAN.T · Jan 9, 2019

Hazzert said:
When it comes to pulling out of a vice a higher helix angle will have less axial lift and would be a better choice. An indexable might be an even better choice with almost no helix.

These are great thoughts, I like where you head is at. but this last one you have introduced variables! Let's assume both toolpaths are using the same tool. which do you think would be less aggressive?

Hazzert · Jan 9, 2019

You can’t remove all the variables because the question is specifically about the variables. A shallower radial pass where only 1 flute and 1 helix revolution is in the cut versus a 1/2D full slotting cut will have vastly different cutting forces and your ears will tell you which is the less aggressive cut.

BRIAN.T · Jan 9, 2019

Well yes I suppose you are correct, I mean to say all other variables removed

Let's say we are using the same 1/2 end mill 10000 rpm in aluminum.

First path is 1.000 axial, .050 radial at 100ipm
Second path 1.000 axial .250 radial 20 ipm

Both paths are cutting at 5 cubic inches per minute.

Hazzert · Jan 9, 2019

You’re really babying those hypothetical endmills lol.

Your .25 stepover cut is the worse cut just because you are using 50% of the endmill and will have higher cutting forces than a wider or shallower cut radially.

BRIAN.T · Jan 9, 2019

Haha yeah, as I was typing it I hated it. Thanks for the insight.

DMF_TomB · Jan 10, 2019

BRIAN.T said:
I've been pondering a few things lately, so I'll ask you guys.

Question one, with all things equal, do you guys step down or step over. Now obviously most of the time there is an obvious logic behind one or the other. But certainly there are other times when either one would do. I personally find myself stepping over. Is there a definitive reason to gravitate towards one of the other.

Second, again variables aside, in a situation where your material removal rate is equal, either by high speed, low stepover or low feed high stepover, which would be less aggressive on the part. Obviously high speed is better for the tool, chip thinning and all, but which is better on the part. Say to keep a part from pulling out of a vise. Im not sure. Any ideas?

Discuss!

.
if you got to remove 0.25 depth and have a surface 10" by 100" most use a facemill.
.
6" facemill taking 5" width of cut and .125 depth of cut often can go 70ipm feed (feed ipt of .010" to .015 is common), 4" FM at 3" width of cut, ,125 depth at 70ipm feed is 26.25 cubic inches per minute converted to chips. often its more a hp and cutting forces limit. not all parts can take a ton of cutting forces and not vibrate excessively.
.
a longer tool in long tool holder doesnt like a lot of depth of cut and low width of cut cause force is directly trying to bend the long holder then longer tools often respond better to less width and more depth of cut. longer insert mill shown doesn't like a lot of side cutting forces. 10" length of cut roughing endmill shown even when 2" dia doesnt like a lot of side cutting forces. sure often cut 6" depth of cut and low width of cut, just not very fast if i dont want to break the $900. end mill
.
usually create a tool database or excel spreadsheet of standard tool setups and cutting parameters and record a range of settings tried and record sudden tool failures. often got not much to do with insert or end mill more to do with length of tool holder
.
very very common on horizontal mill with pallet of 40" to 50" to need longer length tool and tool holders to reach the center of the pallet table

BRIAN.T · Jan 10, 2019

DMF_TomB said:
.
if you got to remove 0.25 depth and have a surface 10" by 100" most use a facemill.
.
6" facemill taking 5" width of cut and .125 depth of cut often can go 70ipm feed (feed ipt of .010" to .015 is common), 4" FM at 3" width of cut, ,125 depth at 70ipm feed is 26.25 cubic inches per minute converted to chips. often its more a hp and cutting forces limit. not all parts can take a ton of cutting forces and not vibrate excessively.
.
a longer tool in long tool holder doesnt like a lot of depth of cut and low width of cut cause force is directly trying to bend the long holder then longer tools often respond better to less width and more depth of cut. longer insert mill shown doesn't like a lot of side cutting forces. 10" length of cut roughing endmill shown even when 2" dia doesnt like a lot of side cutting forces. sure often cut 6" depth of cut and low width of cut, just not very fast if i dont want to break the $900. end mill
.
usually create a tool database or excel spreadsheet of standard tool setups and cutting parameters and record a range of settings tried and record sudden tool failures. often got not much to do with insert or end mill more to do with length of tool holder
.
very very common on horizontal mill with pallet of 40" to 50" to need longer length tool and tool holders to reach the center of the pallet table

I certainly appreciate the insight, and I'm always happy to have people add to the discussion. But I should be clear, this isn't a problem I'm having, I'm not actually looking for a machining solution to something. More of a general physics question. If speed is increased and step over proportionally decreased, what effect does it have on the part. Are cutting forces equal? What do you think?

Thanks

Generic Default · Jan 10, 2019

Cutting forces depend on the spindle torque and the radius of the tool. Most CNC machines have a spindle load meter, which tells you what percentage of the continuous torque available you are currently using. There are also forces trying to pull the tool out of the holder OR forces trying to push it up into the holder. These are proportional to the torque but are multiplied by some constant that depends on their cutting edge sharpness and helix angle. For example, if you plunge the spindle into the workpiece straight down while it isn't rotating, you will see a huge upward force on the tool, even though there is no torque being used to do so.

I think for a given material removal rate with a typical helical flute endmill, the high axial, low radial and high radial, low axial cuts will be close in axial force.

13engines · Jan 10, 2019

Hazzert said:
When it comes to pulling out of a vice a higher helix angle will have less axial lift and would be a better choice.

Ahhh... actually the opposite of this is true. Higher helix, higher axial load, greater chance of vise lift and/or pulling tool out of holder.

Dave

Hazzert · Jan 10, 2019

13engines said:
Ahhh... actually the opposite of this is true. Higher helix, higher axial load, greater chance of vise lift and/or pulling tool out of holder.

Dave

Crap you’re right, don’t know how I mixed that one up.

mhajicek · Jan 11, 2019

Direction and amplitude of cutting forces based on stepover:

Search

Largest Manufacturing Technology Community on the Web

Search

A few machining theory questions.

BRIAN.T

Cast Iron

Hazzert

Stainless

BRIAN.T

Cast Iron

Hazzert

Stainless

BRIAN.T

Cast Iron

Hazzert

Stainless

BRIAN.T

Cast Iron

DMF_TomB

Diamond

Attachments

BRIAN.T

Cast Iron

Generic Default

Aluminum

13engines

Stainless

Hazzert

Stainless

mhajicek

Diamond

Similar threads