mill a Sphere surface

[TheBroWn]

Hi, I'm trying to mill a cavity similar to an interior of a sphere and mastercam did not created G03 code for a complete circle.I use scallop with filter tolerance activated and when I post I have a lot of G01 not much G03 for one circle. In theory, I turn in round around my surface, I must have one G03 with I J for a complete circle and One G01 for linear positioning for the other circle. I have a lot of variation in Z (.0001). What i'm doing wrong??????

Excuse my english!!!!!

Thanks a lot!!!!!!

[Matt Berube]

Which toolpath are you using ?

"Surface Finish Contour" would most likely give the clean output you're looking for.

[Superman]

Originally Posted by TheBroWn I must have one G03 with I J for a complete circle and One G01 for linear positioning for the other circle. I have a lot of variation in Z (.0001). What i'm doing wrong??????

You have done no wrong, mastercam will not output a full circle on a surface op every time, there are gouge checks, cut tolerance and filters that are constantly applied.

Matt has suggested 1 surfacing strategy

also try "Surface Rough (or Finish) Restmill" , set the "flow parameters" in a circular CCW direction and cut from the top ( outside ) collapsing to the centre ( set the big green arrow pointing CCW, and the smaller arrow pointing to the centre, Gaps=follow surface, gap distance= to be set approx tool radius ), "Direction" on tool parameter page may need to be turned ON and used ( BUT, set this area only after the other settings are correct ) this controls how the tool is positioned on the 1st and last cutting point on each pass

( note!!! this "Direction" does not look at your part, it just adds a tool movement at the ends of each pass --- it will gouge, so each pass' endpoint should be checked--- this is where "Gap distance" helps to minimise the number of individual passes

Steve

[neilw20]

Learn to write some g code.
The frustration will go away.
A subroutine can calculate each new Z pass, with parameters.
Full control. No dumb moves. Use your brain, though it still may be generic.

Many CAM packages are an exercise in frustration.
Formula for circle is X^2 + Y2^2 = R^2. if you don't like trigonometry.

[Matt Berube]

Originally Posted by neilw20 Learn to write some g code. The frustration will go away. A subroutine can calculate each new Z pass, with parameters. Full control. No dumb moves. Use your brain, though it still may be generic. Many CAM packages are an exercise in frustration. Formula for circle is X^2 + Y2^2 = R^2. if you don't like trigonometry.

With all due respect neil... it will be far easier to learn the proven Mastercam software than to manually program stuff like this (or anything for that matter). Besides what if something changes ? Tool diameter, stepdown, etc... You're finishing the calculations for the first depth cut right around the time I'm sending the new program to the machine. CAM wins every time.

[neilw20]

With parametric programming all of those changeable thing like tool radius, step over etc are all in parameters.

Set each parameter, and call the generic subroutine.

If it was some strange compound shaped cavity than of course CAM wins, but this is just a damaged hole, and almost trivial.

[TheBroWn]

Originally Posted by Matt Berube Which toolpath are you using ? "Surface Finish Contour" would most likely give the clean output you're looking for.

I use scallop because this is the toolpath with the best finish on mastercam because i can control the scallop.

Finish contour give me the G03 that I want but in the center of the sphere it's not wonderful. I can control the max stepdown but not the scallop. In center this is almost flat. My geometry is a sphere with 60.002" radius cut at dia. 28 3/4". It's about 1 3/4 deep.

With a lot G01 for a complete turn when i try this on my cnc at 150ipm the cnc slow down and the finish is bad.

Other option in mastercam or what cam I must buy to do this kind of job????

Thanks!!!

Martin

[Superman]

Sorry Neil

a cavity similar to an interior of a sphere

is not

just a damaged hole

TheBroWn
Have you looked at Flowline ( I originally said restmill, DUH ), this strategy also looks at cusp heights. Change my original post about Restmill to Flowline and you are good to go

Apologies, after I get my foot out of my mouth.

[TheBroWn]

Originally Posted by Superman Sorry Neil is not TheBroWn Have you looked at Flowline ( I originally said restmill, DUH ), this strategy also looks at cusp heights. Change my original post about Restmill to Flowline and you are good to go Apologies, after I get my foot out of my mouth.

It looks work good. I gonna try this immediatly on my cnc.

Thanks again!!!!

Martin

[Matt Berube]

Flowline is helpful for some situations. My absolute favorite strategy involves using 2 toolpaths on the cut area.

I start with the Surface Finish Contour but I select the "shallow" dialog and "remove cuts from shallow areas". I then follow up with Surface Finish Shallow toolpath to cut all areas missed by the contour toolpath.

This combination approach has provided me with smooth accurate toolpaths for many years.

Flowline will work for the easy stuff but when things get complicated try this strategy. You'll never look back.

[fizzissist]

Originally Posted by neilw20 With parametric programming all of those changeable thing like tool radius, step over etc are all in parameters. Set each parameter, and call the generic subroutine. If it was some strange compound shaped cavity than of course CAM wins, but this is just a damaged hole, and almost trivial.

I can't wait for neil to show exactly how trivial this "damaged hole" is with a posting of the G-code that'll do the trick for some simple example.

Win-win deal. Neil is proven right, and the question gets a novel solution that benefits all.

It's trivial, right? Shouldn't take more'n a couple of minutes.

How 'bout a 2"dia using a 3/8" ball mill?

[fizzissist]

<Yawn><Stretch>
...Comin' up on 6am in Australia right now.

Cuppa coffee (or however you say it in Australian), a couple of eggs, butter your toast with one hand while writing a macro with the other. Standard fare for the chosen few.

It'll take longer for the internet to link up than it will to write the parameters up, set your GOTOs, LESSTHAN or EQUAL TOs and proof the program.

Heck. Neil'll have the code posted here while he's tyin' his shoes! Wontcha, Neil?