Face Mills and Engage?

GreggT · Post by **GreggT** » Thu May 06, 2004 8:26 am

In 2-1/2 Axis Facing w/ a Face mill I am getting ramping on the engage into uncut material. By definition a Face mill only cuts on the periphery or anyway the one I'm using only does. How do I set this up so that all cuts start off of the part yet endup with an efficient tool path and not run into things like part stops that extend above the cutting plane? Everything that I have tried so far ends up in a lot of air cutting and everone knows that that dulls your tools like crazy ;>) not to mention the machine time that is lost. I'm sure I just haven't got my mind around how this is supposed to be defined. Somebody please explain. Looks like we need to be able to define an entry point off the material and an overhang for the first outer cut?

TIA

GreggT

Post by **MecSoft Support** » Thu May 06, 2004 10:12 am

In Face milling, use the Engage in Air settings to control by how much the cutter needs to step out of the material (Linear Extension setting).

GreggT · Post by **GreggT** » Thu May 06, 2004 12:51 pm

This just generates a lot of air cutting. I want to start off the material move into it and then begin pathing. For instance if you have a 3" diameter piece of stock and you want to face it, and are using a 2" diameter face mill, If I select the region that defines the upper edge of the stock and apply a 1" engage/retract in air I get two revolutions around the part before I even start cutting material? This might not be two bad if your cutting AL where your feeds are high and you have lots of time. But if you are cutting SS where the feeds don't even look like the part is moving and in a hurry this will drive you nuts.

If I then construct a circle smaller than the actual material to select I end-up plunging into material (remember this tool only cuts from the periphery, if you ramp it it crashes hard.) I'm looking for an entry onto the facing surface similar to a profiling engage? More cut time less air time.

Also the lower the tool step distance the more air you cut.

I hope you understand what I'm trying to convey. I'm sure this is just a setting that I am not utilizing.

Looks like I should be able to set the entry/exit to Entry>Engage Motiuon>Linear>Height=0, Distance=1.0625, Angle=? and start off the stock?

What am I overlooking?

GreggT

Mark Stacey · Post by **Mark Stacey** » Thu May 06, 2004 10:02 pm

I asked for a similar idea of being able to start tool paths from a defined start point. Response below looks like it is being worked on.
I can't wait for this to happen as I have a box full of face mills that can't be plunged (over load fault on a Z), plus being able to use a pre drilled hole or defined region near a clear edge of the stock would be great for rapid plunge instead of watching a tool slowly spiral down.
Cheers
Mark Stacey
www.cncprototyping.co.nz

Mecsoft reply
For profiling the start point of the curve is the start point of the
toolpath.
For all others, the start point is random. We are currently working on User
defined start points for pre-drilled holes for the next version.

My Question
> Is there any way to set the point the created tool path starts? On some
of my current work I'd like to be able to drill an entry hole and then
always start the tool path from inside that hole.
> Thanks for any advice

DareBee · Post by **DareBee** » Fri May 07, 2004 5:30 am

This had me really pissy the other day when I was using horizantal roughing AND working on a rush job.
My part setup was too soft to take more than 50% of my cutter( It took about 80% of my cutter to mill the stock). When I set the step over to 50% it took 3 paths around my part the first cutting air! By my calculations 2 cuts at 50% is greater than 80%.
Of course my step down was about 20 rounds.
1 air cut per round!

GreggT · Post by **GreggT** » Fri May 07, 2004 7:52 am

Cutting air blows ;>)...

GreggT

obwan425 · Post by **obwan425** » Fri May 14, 2004 3:52 am

I have used the curve machine under 3d to help alleviate some of the problem..I create a boundary(or use geometry provided)turn it into a surface ,flat plane, use the along curve machine,give the ammount to cut on the side of curve a huge number so it completely fills the area to be cut,use a large lead in,crunch and reverse the toolpath so the lead starts on the outside instead of the inside. What I get is a toolpath that starts outside the boundary(off stock) moves in and makes its first pass on the boundary I created and moves in from their.Then I will also instance the toolpath in z to achieve the required depth. Crazy but it works and saves me the air pass..Cuz yes that sure does make a cutter dull,,verrry dull!

GreggT · Post by **GreggT** » Fri May 14, 2004 6:56 am

LOL

Thanks for the tip I will give this a try. Love that machine shop humor too. To bad this isn't simpler.

GreggT

BJMAUCH · Post by **BJMAUCH** » Sat May 22, 2004 6:43 pm

I know that this sounds rediculous, but I am using 2.5D engrave with the on condition to draw a path that I want the tool too follow to get to the material and to cut it. Although this does not give me diferent feeds of engage and cut, at least I can control where and how the tool gets to the cutting area.
P.S. I rename the engrave MOP to say Exact Path so I don't get the phone call about can't be right engrave with a face mill.

Barbara

obwan425 · Post by **obwan425** » Sun May 23, 2004 5:09 pm

bj,

Definately not rediculous!!!I've done the same thing before works fine!!Not saying that this issue shouldn't be addressed,but its nice to see people sucking even more out of the software than was originally planned...

Greg