1/4 radius with 1/2 endmill?

[poconnor]

Hello All,

I was cutting some mating puzzled pieces of plastic with a 1/2" endmill and when I took them off the router the radii didn't mate properly. It had 2 1/4" radii that were rounded out. The only way I could get them to mate properly was to change the radius to .260. We are new to Mastercam and we never had this problem with our old CAM software. Can anyone tell me if there is a tolerance in Mastercam that I can change to alleviate this problem? or is this a post or control issue?

 

Thanks in advance!!

[mold100]

Not to ask a stupid question or anything is it possible your 1/2 inch cutter is undersized, maybe a re-grind? I am not really familiar with routers but a .01 mistake is alot even with open tolerances.Or accidentally had stock to leave set.

[poconnor]

"There are no stupid questions, just stupid Managers"

 

The endmill is brandnew out of the box. Everything else was cut fine it was only the 1/4" radius that wouldn't come out right. I thought it might be the control just going too fast into the corner and rounding it out but our supplier assures us that the High-speed cornering software we have installed would slow down way ahead of time to take the corner.????????

[Brendan P]

Not sure but did you maybe have a value in your X Y stock to leave on? Are you using cutter comp.

and have a value stored in the control?

[poconnor]

x,y stock to leave is 0.00, cutter comp is on computer. This is why I'm wondering if there is a tolerance on what size radius a cutter can cut with cutter comp on??

[Eric S.]

Is this an inside rad? I almost never get a good result miling an inner rad with the same size e-mill. If you can I have found using a smaller e-mill makes much nicer corners. Finish and size.

[cadcam]

Poconner try turning of the Roll all conners in the second paramater page.

 

this might be causeing the issue with this machine.

[poconnor]

I'm trying to avoid using a smaller e-mill. 1/2" is the standard cutter we use on our machine for profile finishing. I just checked in the parameters and I had corners set to SHARP do you think if I change it to NONE that will work????

[TheePres]

Not familiar cutting plastics. But as material to the left of cutter is being climb cut, material to right is convential cut. If there is any deflection, it would be apparent on right (.25 rad) side only.Just a thought.

[cadcam]

Poconner this is a huntch truthfully but I have seen this happen on some machines before.

 

If you can take trial cut.

[poconnor]

OKAY! Thanks CadCam I'll give it a shot. Thanks to everyone else for the help too!

[CNCme]

Good day

 

Welcome to the forum

 

Are you talking a little or alot

Most endmills, and most carbide are .001 to .003

undersize out of the box.

sometimes plunge the corners or slow the feed

to clean corners.

 

HTH

 

Tony G

Unemployed Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

and coolant and chips are like the enemy

under your boots as you advance in the

Manufacturing Battle.

__________________________

[poconnor]

No I'm talking a lot. It's giving me approx. a 7/16 rad. And If I change it to a .260 rad it cuts it .260 bang on the cash! I'm going to try CadCam's suggestion and turn roll around corners off. I hope this works, cause if not I'm going to have to add a lot of tool changes to my programs or re-draw all my geometry.

 

I even tried lying to MasterCam and telling it the cutter was only .497 and it still didn't work until I changed the rad. to .260. This is why it sounds like a tolerance thing to me. Because even at .259 it didn't work but as soon as I went to .260 it worked great????????

[Eric S.]

Have you tried to make a spring pass to see if there was any deflection? When the 1/2 e-mill hits the 1/4 rad it will tend to deflect because there is a much larger cuting surface. It may help just to rule it out.

 

Eric

[Scott Bond]

Hi Poconner

A new to you Mastercam will also have a new to you post. Is it possible the your post is giving your router a look ahead code.?

(Like A G8 on a Fadal)

Have you set the old system and new system nc code side by side, and looked to see if the actual numbers are .010 differant?

 

Hi Jay ,are you feeling better?

 

[ 04-17-2003, 04:03 PM: Message edited by: Scott Bond ]

[Nominal]

Sounds like normal tool deflection trying to slam into a 90 degree corner. I'll bet when you use .250 rad geometry with a .250 tool your resulting nc code is purely linear, but when you change the rad in your geometry to something bigger than the tool geometry, mastercam spits out a arc move. Don't forget that without an arc move on your inside corners there is a definate change in velocity since one axis has to go to nearly zero velocity ( not actually zero since there is a following error ) and the next axis has to take over from zero ipm. There is a time factor involved, enough so that the force vector is not constant and a deflection occurs. I never generate inside radii with a tool of the same size unless its some crap nobody cares about. ( and even then I don't think I'd do it just cause it's gonna look like s%*t.) Also....

 

quote:

---

but our supplier assures us that the High-speed cornering software we have installed would slow down way ahead of time to take the corner

---

My guess is that its only going to be aware of a "corner" if there is an arc move in the program. Otherwise what constitutes a corner? It would be slowing down everywhere an axis changed otherwise.

[cadcam]

quote:

---

Hi Jay ,are you feeling better?

---

Alott better then on monday that is for sure.

Thanks for asking.

[Rick Damiani]

quote:

---

I even tried lying to MasterCam and telling it the cutter was only .497 and it still didn't work until I changed the rad. to .260. This is why it sounds like a tolerance thing to me. Because even at .259 it didn't work but as soon as I went to .260 it worked great????????

---

I beleve the source of the inncorrect radius is deflection, as others have mentioned. On the above, though, I can maybe shed some light.

 

In your post, there is a value called arccheck with associated length and angularity tolerances. If those tolerances are set too large, the small arc moves generated by the toolpath will be replaced with line moves. With the MPFAN post, I was able to get the kind of behavor you are seeing (arcs at a R of .260, no arcs at .250 to .259) by setting arccheck to 1 and setting the length tolerance to .015.