Circle mill problem?

[Brendan P]

Good morning gents,

I would like to cut a 3.0" circle in a plate that is approx. .250 thk.

Using a 1.0" endmill.

I have tried to use contour,but can't get it to work the way I want.

I want to start in the center,move over in "X",mill the circle leaving .020 to finish.

But I don't want a "retract" on "Z" for my finish pass.

I want it to complete the circle,then nove over the .020 and swing the finish pass ,keeping "Z" down.

 

Please help!

Ps I have always edited my code to get these results,and I'm tired of it.

[Lathe-Mill]

check the box for "keep tool down"

[Lathe-Mill]

on the lead window, check lead at entrance only and lead at exit only

[Brendan P]

I tried this but mastercam doesn't like to "keep tool down" using a contour path.

[robk]

Hey Bucket, it sounds like you're using contour toolpath and not circle mill.

 

Rob

[Brendan P]

What I'm saying is that before it runs the finish pass,it wants to go back to the starting point instead of just moving over and swinging the finish pass.

 

I tried both,but cant get it to work right.

Can it even be done in contour??

 

[ 10-14-2003, 11:51 AM: Message edited by: BUCKET HEAD ]

[Lathe-Mill]

circlemill has the multipasses option, keep tool down, and for finish pass leave the .020 you want

[mayday]

Try multi pass Bucket, leave the .02 for finish that way, I think it will leave the tool down

Oh, do this with contour

 

[ 10-14-2003, 12:02 PM: Message edited by: MayDay ]

[robk]

I see what you mean. Editing the NCI is about the only option I see right now.

 

Rob

[Lathe-Mill]

bucket i think you best bet is circlemill, multipasses, 1 rough pass, 1 finish pass of .020, check tool down, finish at final depth.

[Fig sign]

Depth cut order must be by depth not by contour

Keep tool down must be both in depth and multypases

[Brendan P]

OK.

I put a sample file on the FTP. Mc9 folder

It's called circle test.mc9

(this is not the actual file I'm using but will work as an example)

 

Now when the tool goes to do the fin. pass,it wants to move back to the center first.

 

WTF!!!

I would like to start in the center of the circle.

Now do you see what I mean?

 

I dont know where you guys are getting the "depth cuts crap"

The plate is only .250 thick

1 shot on depth!!

 

[ 10-14-2003, 12:21 PM: Message edited by: BUCKET HEAD ]

[Lathe-Mill]

bucket, circlemill will give you that option, start at center

[robk]

Bucket,

 

Pocket toolpath worked here, still had to move my first point in the NCI. Chain the arc only... No points.I gave it 2 finish passes without any rough with .02 spacing. Small lead in & lead (5%) out with a 90 deg. sweep (if using carb. insert cutter). Right click the NCI in the operation manager and move the first point to the center of the arc.

 

Rob

 

[ 10-14-2003, 12:30 PM: Message edited by: robk ]

[Lathe-Mill]

bucket, that is exactly what i ment, i see what you want, you dont want to go back to the center , right?

i think mastercam wants to finish the rough pass completly going to the center (start and finish point), then finish it

[Lathe-Mill]

in that case, dont start at center

[Brendan P]

quote:

---

bucket, circlemill will give you that option, start at center

---

Dowload the file and swow me then please.

 

Rob,the reason I don't want to use pocket,is because I just want to go around,and let the slug fall through.

Too much wasted time pocketing out the center.

Where's the man with 2 first names when you need him?

[robk]

Sorry I can't help ya. No FTP access... Security reasons you know

 

Rob

[Lathe-Mill]

circle mill, starts roughing at center and finish at center then does same with finish pass, uncheck the start at center option, wont go back to center but starts close to the dia. and finish how you want it. sorry pal. dont see other way

[mayday]

Bucket, take a look ftp site circle new

[cam-eleon]

check file: circle test2 on ftp

It might be OK

[Lathe-Mill]

i got it !!!

 

contour, multipasses,rough passes 1,finish passes 1 (.020),tool down, at final depth.

lead in, perpendicular (50%)

check the enter on first cut only and the exit onlast cut only, .

 

work here man, hope it does for you!!

[Brendan P]

Give me a few to try it out.

I will let you guys know.

Thank you

[Brendan P]

Tatalo,you did get it.

Circle test 2 was exactly what I was looking for.

Circle test new was the same also,with different lead in/lead out.

 

And rob,yours would work,and it was a sneaky way of doing it,I didn't thik to try your way.

 

Thank you guys for bailing my A$$ out again.

You guys a awesome!

[Lathe-Mill]

I guess I am learning , Am I?...