Spiral Pocket Question

[Andy]

I drill a .5 hole.

I want to counter bore .625 dia .25 deep with a 3/8 end mill.

I want to spiral out and take .007 per pass at

full depth (.25) until I get .625 dia.

However, I do not want to cut air for the first

.124 of dia.

When I use spiral pocket it starts the spiral at the center an cuts air for the first bunch of the spiral.

 

How can I cut with spiral path and start at near .500 dia and spiral out to .625 dia?

 

Thanks,

[Mick]

I can see two ways to do this:

 

1) Use contour, and use a lead in/lead out, if you need to use a 3/8 cutter. Use multi passes, with a setting with something like 9 passes at .007

 

2) To use the spiral pocketing toolpath, you need to use a small cutter, like a 3/16. Draw a .125 circle in the centre, and select that, together with the OD of your counterbore, and select spiral inside to outside. Should work fine, though I would probably cut the across cut distance back to something like .004. That really depends on the material

[Slixmix]

I like the circle mill toolpath for something like this. I like the start at center feature. toolpaths - next menu - circ tlphs - circle mill. If you choose a point, you have to input the diameter of the hole. If you click on an arc, it knows the diameter. Works well for me

[Andy]

Thank you for all the answers,.

However, what I am trying to do is have a spiral toolpath that "continuously" cuts out to the finish size at approx .007 tool load with no lead ins or side steps and does not cut air and uses a 3/8 em.

Contour , goes in and out of the cut with leadin leadout.

Spiral pocket with 2 circles requires a smaller end mill.

Circmill , goes in and out of the cut.

There should be someway to do this.????

Thanks,

Andy

[Rick McAllister]

What is the material?

[kathy]

I also need do machine a pocket in a similar way. My starting point isn't in the center of the pocket, so I have to cut a 'dummy' pocket to clear out the core to an area where the 'real' pocket begins. Alot of extra cutting. So I'm willing to try all suggestions!

 

Kathy

[Guest CNC Apps Guy 1]

Not to play devil's advocate or anything but why do you have to do this this exact way/ Just curious that's all. I would not like the dwell marks that not leading in/out would leave.

[MichaelJ]

Do a .124 step over then 9 finish pases at.007 then that should do it if that is what you are looking for

 

[ 12-11-2002, 03:02 PM: Message edited by: MichaelJ ]

[kathy]

James,

 

I'm shearing off core sections using a valve stem cutter. The tool is buried under the core material. The cutter diameter is 1.0 but I can only shear off about .3 cut at a time. I cannot move the tool throught the core as the shank will bind up. I can e-mail you a file if you'r interested.

 

Kathy

[Guest CNC Apps Guy 1]

Kathy,

 

You have my work e-mail right? Send it there.

[Mick]

I dont get it. By having a central island, and an outer boundary, the true spiral pocket method would do exactly what is required. Or maybe I'm missing something.

[Camdude®]

i like nick's idea of placing an island at the center of ther pocket. that should force the tool

cut between the two contours...

[Andy]

I actually could use any of the suggested methods to do my job. And, I actually am using the finish stepover .007 method.

But, ideally,I am just curious if, given my conditions above, can a non interupted true spiral be accomplished?

That is: starting with a 1/2 hole spiral out with no stepovers using a 3/8 EM and not cut air.

 

PS: There is not room for an island contour in this case.

 

Andy

[ROB]

have you try contour ramp with perpendicular

entry/exit ,that wont cut air!

[camguy]

Andy, take a look at "spiral.mc8" file on Jays ftp site under mc8files directory. I just used the "spiral" chook, 1 revolution. break the spline at the midpoint, create two arcs on top of the splines. delete splines, offset the arcs .007.

In toolpaths chain the arcs from the inside out and select your .625 arc last. lead in off, lead out perpendicular .063, arc "0". save this and import into your files anytime. use the same method for different size holes and c'bore sizes and create a library to speed things up. hope this helps

[Andy]

Rob,

Yes, Contour ramp works good also, but I want to cut with the side of the em and feed spirally out not down.

Camguy,

I will try those suggestions, but not tonight. I will respond after I try it.

 

Thanks guys,

Andy

[gcode]

Create a spiral toolpath from the center

with the .007 step.

Backplot and save as geometry. Post ghost or delete this operation.

Trim the saved geometry that is cutting air.

Create a new op chaining the saved/trimmed geometry. No cutter comp and 0 incremental depth of cut.

Its a little exta work, but you have total contol.

[Andy]

Hey gcode,

That sounds like that will work good I will try it. Too bad it isn't easier.

Thanks,

Andy

[gcode]

Let me know how it turns out.

[steve f]

Hi Andy,

 

If you're looking to create counterbores with very little load on the tool, I've found that using a threadmill toolpath works well for roughing this kind of feature. Setting the pitch around .01" for this instance allows you to get away with feed rights considerably higher than you might expect. Also the tool load is constant through out the entire cut and chip evacuation isn't as much of a problem than having the cutter buried to full depth and taking all cuts radially.

 

Good luck,

 

Steve

[rchoward]

sorry guys gotta side with rob... cbores rip with a 2d ramp move use 4-7deg leave a finish pass on xy nothing on z

 

then a standard 2d contour to finish with overlap and lead in lead out

 

use a 2fl stubby and go for it

 

if u ruff drill the cbore carefully ucan go right in there wihout any ramp and finish especially in plastic/alum... on more tool but how fast is your changer... drills are cheap

 

one more thing make sure your machine supports helical moves or else u are going to crank out alot of code

[Rick Damiani]

quote:

---

I drill a .5 hole.

I want to counter bore .625 dia .25 deep with a 3/8 end mill.

I want to spiral out and take .007 per pass at

full depth (.25) until I get .625 dia.

However, I do not want to cut air for the first

.124 of dia.

When I use spiral pocket it starts the spiral at the center an cuts air for the first bunch of the spiral.

 

How can I cut with spiral path and start at near .500 dia and spiral out to .625 dia?

---

I see lots and lots of really complicated ways to accomplish this in this thread, many of which seem to revolve around creating odd-ball geometry. Lotta work.

 

Me, my first thought was - well my first thought was pretty dumb so let's forget that one. My second thougt was to try a trimmed toolpath, and that seemed to work well. Here is how I did it:

 

1) Create a true spiral pocket tool path with a .007 step-over using a 3/8" mill on the .625 dia hole.

 

2) Draw a .124 circle at the center of the .625 hole.

 

3) Select Toolpaths-Next Menu-Trim and select the .124 circle.

 

4) Pick a point outside the .124 circle.

 

5) Select the pcket from step 1.

 

6) And Bob's your uncle.

 

You can, if you wish, fiddle with the graphical toolpath editor to add a lead-in move, create a point toolpath, or use a reference point to make sure that the tool's initial approach is a safe one.

 

I'll post the MC9 file if anyone is interested, but the path is pretty simple to reproduce if you follow the above steps.

[Scott Reiner]

Nice answer Rick, I should have read your post before, I came to the same answer as you. Ricks suggestion works like the wind. Scott