Pocketing vs Circle Mill

[George_Gerhard]

Just curious what makes you choose one over the other, is it just island avoidance, and the entry methods?

Thank you

George

[robk]

Circle mill is just it--circle mill. You can mask on arc and not chain the geometry. You also have the option of selecting it by points and entering the dia. of the circle. You also have the option of starting the tool in cener of arc. Cicle mill is much quicker for the right application.

 

Rob

[George_Gerhard]

Thanks Robk I am trying to get different opinions

George

[robk]

 

Where are you in CT?

 

Rob

[George_Gerhard]

Shelton

[Guest CNC Apps Guy 1]

I prefer contour/pocket because you get more control over various aspects of your machining strategy. I more often than not, use ramp contour for the consistent finish it gives as opposed to the steps you see (but don't feel) from just a step down method.

 

JM2C

[George_Gerhard]

Thanks James

Are you saying you use pocket then contour ramp to finish?

regards

George

[MetalMarvels]

In using both methods, I have to agree with James. You have much more control in the pocket/contour method. I have had some amount of difficulty hitting my target size with circle mill, but it is really great for those "wide-open" tolerance "fast" holes that are really too big for a drill (or you need a flat-bottomed hole). Also the ramp down on finish gives a superb finish.

 

JM2C

 

[ 10-06-2003, 06:17 PM: Message edited by: MetalMarvels ]

[connormac]

I had never thought about Ramping on finish pass. How much do you leave on for finish pass and how fast do you feed down.

 

[ 10-06-2003, 06:37 PM: Message edited by: connormac ]

[Guest CNC Apps Guy 1]

The answer depends on the tolerances involved. Wide open (±.010" or more) I'll leave like .03 and feed around 150 IPM. If less tolerance, I generally cut the feed and stock to leave by 50% or so. Our Mori's will hold roundness of .001 at 75 IPM on like a 1.500 diameter or more using a .500" E/M

 

HTH

[Guest CNC Apps Guy 1]

George, that depends on the hole size. I don't use drills larger than .750 so if it's larger, I'll drill the center out, rough the pocket leaving stock then finish it up with ramp contour.

 

Depends on how I feel that day.

[George_Gerhard]

Thank you James

[cadcam]

quote:

---

Depends on how I feel that day.

---

So how doy you feel this day?

 

James a little note:your mail is back up sorry about the down time.

 

Jay

[connormac]

Thanks James,

 

I'll try it and tell my wife about it also.

[Guest CNC Apps Guy 1]

quote:

---

So how do you feel this day?

---

Today is a rough day. Hopefully it finishes well.

[cadcam]

quote:

---

Hopefully it finishes well.

---

I hope it does to..I'll give you a ring towards the end of the week to see how it all went.

[crazy^millman]

It depends on the material the depth of the hole and the tool I got to use to do it. I like circle mill on deep holes cuase I can use entites as a control instead of manual and it works on points as well this way and it will do like a pecking routine to circle mill the hole when doing stuff 10x tool dia real big help to clean out the chips. I haved used the other but I am an old Mazak User and Mastercma is alomst the same when it comes to do it in the way I am use to for so many years with the aspect of circle milling.

 

Crazy Millman

[Andy]

Hey Millman,

What do you mean by entities instead of "manual"?

Andy

[crazy^millman]

Well when you got to the toolpaths/next menu/circ tlpths/entities/ then you have the follwing options:

Unselect

Chain

Window

 

Area

Only

All

Group

Result

Done

It kinda goes like everything else here. The unselect you know the chain is just like it says. Window is very powerful if you are doing a bunch of holes even if they all different sizes it will do them all. Area I have not used help says this:

quote:

---

The Area selection option of the Entity Selection menu provides a technique for selecting multiple nested shapes with a single mouse click.

Instead of drawing a box around the entities to be selected (as in the Window method) Area selects closed boundaries around the point where you click the mouse.

To select all of the shapes within a closed boundary, choose Area, Options, and check the Infinite nesting in area chaining box.

---

ONLY this is my favorite but requires a little up front thought. I create all my points in the center of the arcs on a different layer but do what you like. I then use points as my control I also use arcs when I have circles they have to be closed or it will grab the quandarts. Group is another one I dont use here is what help says:

quote:

---

Groups allow you to gather entities into a single unit for selection. When working with groups, Mastercam performs a function on all the members of the group as a single unit. This prevents you from having to select entities individually when you want to perform a single function on multiple entities. The Entity Selection menu provides the Group selection method for this purpose.

When performing a transform function (from the Xform menu) Mastercam creates a temporary group from the originals and a result from the transformed entities. These system groups are listed in the Groups dialog box along with any groups that you create. However, the system group and system result only stay in effect until you use the Screen, Clr Colors option or perform another transform function.

 

Mastercam requires each group to have a unique name. Duplicate group names resulting from merged files have a + sign appended to the name. Mastercam automatically creates unique group names, such as T1, T2, etc., for groups resulting from Create, Next, Pattern

. You can also assign your own names in the Groups dialog box.

---

The next is result which shows you what you have come up with entities. The last of course is done.

 

Now here is what I have found to be the big different between grabbing things this way verse the Maunual selection way. Mastercam will automatically do a circle mill cut then do a complete retract to the retract plane if that is only on or to the clereance plane. I compare it to pekc drilling but doing a circle mill toolpath.

 

I have put up an example call CIRMILLPECK in the MC9 folder on the FTP. if you look at the code and the Backplot is pecks just like a G83 peck drilling cycle. I then say you try it with Manual and the try it with entities and see the different between the 2 different toolpath.

 

Note you can make this way stay down if you say keep tool down in the depth cuts dialog box. Like I said earlier if doing deep holes, real stringy material, or hard to machine material that have a thendency to work harden it is a great tool to clean out chip and allow the stringy chip to clean off and to get coolant to the tool.

 

I am sorry for the long explantion but I hope some cut and paste this for their help books.

 

Crazy Millman

 

PS CBORE CRAZY in the MC9 folder is antoehr example using circles as control.

 

[ 10-06-2003, 11:21 PM: Message edited by: Millman^Crazy ]