3D Contour Help

[Ocean Lacky™]

I have a 3D Contour that I want to mill with a 1" Ball Mill. The contour is a curve at the top edge of a 1/2 radius surface. I programmed with comp set to center of tool and it backplots fine, but it posts out 1/2" high.

 

I know it's something simple, just don't do this often enough.

[Zoober]

I have found center comp to do that.......... try tip and see if that helps

[Ocean Lacky™]

tip works but it will undercut the near vertical portions of the contour

[3R!< W3NG3R]

Why does it undercut? I only use tip. haven't found a use for center.

With tip I have never had a problem with contour undercutting. Another setting maybe.

[Ocean Lacky™]

I don't know for certain that it does undercut, but it 'appears' to be a considerable amount in Backplot.

[Troy Gossett Indepak Inc.]

I made myself an example file because I never remember how I did it last. 3DCONTOUREXAMPLE.MCX

 

In case the link doesn't work it is here: Mastercam_forum/All_NC_programs/3DCONTOUREXAMPLE.MCX

[88Matt]

Ocean,

It will undercut as u go vertical. it is not doing the trig to keep the tool tangent to the curve. It is just looking at a point on the tip.

[Thee Rickster ™]

It is the type of curve you can create the surface

and project a contour path on the surface?

[Müřlıń®]

Ya you have to do a surface finish contour and use your curve as the boundary.

 

That way the surface is figured in...

 

but if your z varies, you will have to use a pencil path or a blended/projected...

 

I guess you could also do a scallop and just use the outer boundary as well...

[TKDBB]

"I have a 3D Contour that I want to mill with a 1" Ball Mill. The contour is a curve at the top edge of a 1/2 radius surface. I programmed with comp set to center of tool and it backplots fine, but it posts out 1/2" high."

 

"I know it's something simple, just don't do this often enough."

 

I assume you did set your tool length offset to the center of the ball?

[Ocean Lacky™]

It's a 4.75" deep pocket with vertical walls. the bottom is not flat. I was trying to cut the walls with a 1"ball endmill while following the contour of the bottom. I ended up cheating a bit by offsetting Z at the machine until I got a radius at the bottom I could live with. Fortunately, it's not fussy, more cosmetic than anything else.

[HT]

Ocean ,try this

1. 3d contour with 1.0 dia. ball nose

2. Comp set to tip

3. Z stock to leave = -0.500

[88Matt]

HT,

That won't help with gouging the vertical walls.

[Troy Gossett Indepak Inc.]

Offset the contour by .5 away from the wall then

comp set to center and z-.5 if you don't offset the contour and just set the Z the cutter will move to center on the wall giving you a .5" gouge.

 

Were you able to look at my example?

[88Matt]

Troy's way will work fine. I just don't like setting my TLO's to the center of the radius. To me it's just another variable that makes it easier to crash. I would prefer the surface project method.

 

HTH

[Müřlıń®]

I would just lie about the toolsize...

 

Then it would stay off the walls...

 

Better still...

 

just leave stock....stay off the bottom and the walls.

 

 

Then you could do a shallow and give it an angle that is great enough to compute the whole surf.

 

Go from inside to outside and save geometry.

 

copy the last couple passes and you will be good to go...

 

you can then do a contour on those and import the NCI into your op to verify...I have done this many times...

 

course there are always more way to do something

[Thee Rickster ™]

Ocean,

 

Can you share this file for us to give a try?

 

Email me if you wish

 

Rick

[billystein]

Offset the contour by .5 away from the wall then

comp set to center and z-.5 if you don't offset the contour and just set the Z the cutter will move to center on the wall giving you a .5" gouge.

 

i like this method but i will translate z-.5 or whatever the radius on the tool is. what you are doing is creating the center geometry and move it to the tip.

 

if you really want to get creative then use this method with a bull em. it really is the same. you offset geo, move to the center of the tool then down the radius amount.

[Ocean Lacky™]

For anyone interested, I put the file up on the FTP...9509-3D contour.mcx. I'm thinking setting the TLO to Center would have been the way to go.

[Thee Rickster ™]

Ocean

 

In fartcam I used to offset the geometry 1/2

the dia of the ball and transform it down

1/2" the dia.(mimics toolpath)

 

Then toolpath the tip on the contour

 

 

(Which in turn is how the toolpath is suppose to

perceive the offset of geometry anyways.)

 

HTH

[Müřlıń®]

Hey Ocean you using a negative insert?

 

or a positive one that will ramp down?

 

That will determine the strategy used to clean up that raidus..

 

First off I will close off that open side where the bender is so that the toolpath will process easier...

[billystein]

the reason i don't use center is that if you change to center you have to change back to tip at some point. it is to easy for me to not notice that setting because i never use it. no big deal until you come back to this file next month and forget to look at it. moving the geometry keeps the program good when you come back this file later. you can always isolate this geometry to a level with a note.

 

this is the way to program 3 axis with level 1 or level 2. you can do many operations that normally require surface toolpaths.

[Ocean Lacky™]

Murlin,

 

Actually, I used an old-fangled 4 flute highspeed ball endmill...the vertical wall was more critical than the radius at the bottom (Die Lock with .004" clearance per side). The radius inward is just gutter. It's only a forging die, not a Swiss watch.

[Müřlıń®]

Endmill is even better...

 

They use those Mitubisi negative inserts around here that dont ramp worth a crap because they have like zero chip clearance...

 

So ramping down busts up the inserts where the Iscar positive will gouge down to China with no problem...

 

I know you are just trying to clean up the radius so as not to have to bench so much...

 

I am processing one now take a few...

[Müřlıń®]

ooops