Contouring with 1/4 in ball end mill from bottom to top

[zachdem1000]

Struggling to get exactly what I want for this contour. I'm cutting a countersink for a 5/16 clearance hole in stainless steel(.332 D at the bottom & .635 D at the top). I'm cutting the clearance hole first and then countersinking. 

I've experimented with different 3D tool paths and found that contour works best for what I'm doing since it allows you to arc filter and and cut from the bottom up. 

The step up is set at .015 and ideally I want the tool path to have a radius at each step up so the code isn't so long.  

 

Anyone know of a better way to set up the arc filter or a better toolpath? Thanks!

[scottm085]

Here is what I generally use.

[Aaron Eberhard]

4 minutes ago, scottm085 said:

Here is what I generally use.

This matches my settings, although I generally enable XZ & YZ arcs as well. 

Also, for something like this, a Flowline toolpath works great.

[cruzila]

2D contour, set the angle and go......I would set it at .005-.007 step with a high feed because of radial chip thinning. Or just get a big c'sink tool

 

Or rough it 2D contour big steps and finish with the c'sink. Many times, there are other factors that drive these decisions related to individual tastes and customer preferences.

2D taper.mcam

[JParis]

2D Swept

[TFarrell9]

5 hours ago, Aaron Eberhard said:

This matches my settings, although I generally enable XZ & YZ arcs as well. 

Also, for something like this, a Flowline toolpath works great.

I also like flowline for this, though I generally tend to use waterline instead (just more control) and set it to spiral.

sub-.0002" tolerance on the arc filter for a countersink is pretty wild, I'd also set it to .001" as previously suggested.

[gcode]

Blend works well too.

Draw a circle on the big OD of the c'sink and a point in the center.

Select the conical surface as your drive surface.

Then chain the circle followed by the point

Use dept limits to control  where it starts and finishes

[crazy^millman]

Remember Mastercam filtering has been and is still tore up from the floor up. Simple test make a 100" diameter sphere and then flowline the sphere with a 1" ball endmill. Throw as many filters as you want at it. See which one gives you only 100% arc moves for the cuts. I have ran this test on every X version since X came out. Not a single version can give me 100% arc using filters. I have backplot the toolpaths make arcs and run a Contour toolpath with no comp and guess what the code never matches. This is the math test the filter fails every year. Just ran into using 2D Peel on a 40 year old machine. Wanted the smalest amount of code possible. What does anyoen think gave me the smallest code out Mastercam?

.

.

.

.

 

No one willing to guess what filter settings gave me the correct code?

 

.

.

.

.

.

 

Come on no one is willing to guess? No filters gave me the best code. Now no filters on a 3D toolpath doesn't behave the same as with filters. Let me repeat that no filters on a Peel mill toolpath gave me the cleanest code with all the arcs and line movements. With a filter it was junk IMHO. Now 3D toolpaths don't behave the same way. Screams fundamental math problem somewhere and for over 15 years no one has dug into why. I am the crazy person on the forum so I guess there is that to consider I mean we all know math is about feeling and mood swings. No way I should expect a G2 and G3 to be just that they can be whatever Mastercam decides it wants them to be and just keep your head down and go along with the idea it is good and it is good.

[Kalibre]

I'll usually use a Thread Mill path.

Keeps the tool engaged instead of repositioning like contour.

Don't end up with the transition lines like a surface path and control comp for any required size adjustments.

Can also back bevel undercut bores.

[Matthew Hajicek - Singularity]

The old "wireframe" surfacing toolpaths have always given me very clean code when I needed it.  Running modern machines I don't need it though.

[gcode]

This thread made me think of this very useful  old Camistructor video.

I always forget these toolpaths are available.

 

 

 

[riverhunter]

On 3/30/2024 at 7:02 AM, crazy^millman said:

Remember Mastercam filtering has been and is still tore up from the floor up. Simple test make a 100" diameter sphere and then flowline the sphere with a 1" ball endmill. Throw as many filters as you want at it. See which one gives you only 100% arc moves for the cuts. I have ran this test on every X version since X came out. Not a single version can give me 100% arc using filters. I have backplot the toolpaths make arcs and run a Contour toolpath with no comp and guess what the code never matches. This is the math test the filter fails every year. Just ran into using 2D Peel on a 40 year old machine. Wanted the smalest amount of code possible. What does anyoen think gave me the smallest code out Mastercam?

.

.

.

.

 

No one willing to guess what filter settings gave me the correct code?

 

.

.

.

.

.

 

Come on no one is willing to guess? No filters gave me the best code. Now no filters on a 3D toolpath doesn't behave the same as with filters. Let me repeat that no filters on a Peel mill toolpath gave me the cleanest code with all the arcs and line movements. With a filter it was junk IMHO. Now 3D toolpaths don't behave the same way. Screams fundamental math problem somewhere and for over 15 years no one has dug into why. I am the crazy person on the forum so I guess there is that to consider I mean we all know math is about feeling and mood swings. No way I should expect a G2 and G3 to be just that they can be whatever Mastercam decides it wants them to be and just keep your head down and go along with the idea it is good and it is good.

Wasn't that about the same time mastecam stopped creating its own tool paths and began purchased them from a (unnamed ) 3rd party?   makes a lot of sense why legacy paths do not have or need a filter.  New tool paths are point to point and need the filter i believe.

[gcode]

1 hour ago, riverhunter said:

Wasn't that about the same time mastecam stopped creating its own tool paths

The ModuleWorks 5X toolpaths are licensed from ModuleWorks in Germany.

Everything else is created and maintained by CNC Software.

That includes all the old legacy 5x toolpaths, 2 and 3d contouring, pocketing, high speed surfacing,  drilling, 2 and 3D dynamic roughing and finishing and all lathe toolpaths.

To Mastercam's credit, the toolpath filters are much better than they used to be.

It used to be a little scary using the filter because you never knew when a filtered toolpath was going to get a glitch and blast through a wall

or an arc was going to wipe out a part with a 358° move  instead of the desired 2° arc.

Filtering used be scary, I worked with people who would not use filtering under any circumstances... even if they had to break a file into multiple programs to get it in the machine.

Filtering is much more reliable and safer than it used to be.

It has been years since a filtered toolpath bit me.

 

 

[cruzila]

On 4/5/2024 at 12:19 PM, gcode said:

 

It used to be a little scary using the filter because you never knew when a filtered toolpath was going to get a glitch and blast through a wall

or an arc was going to wipe out a part with a 358° move  instead of the desired 2° arc.

Filtering used be scary, I worked with people who would not use filtering under any circumstances... even if they had to break a file into multiple programs to get it in the machine.

Filtering is much more reliable and safer than it used to be.

It has been years since a filtered toolpath bit me.

 

 

We have one machine (older machine) that will do the 358 degree side every so often. I understand it is a function of the machine controls ability to calculate and not really filtering per se. I will go back and change the min arc or step over a tiny amount and it generates code that works

[bird2010]

Can you accept 2D toolpaths?
2D tool paths have NC codes for shortest and concentric arcs...
It can also be done from bottom to top...

 

 

 

[bird2010]

17 minutes ago, bird2010 said:

Can you accept 2D toolpaths?

Oh...I just found out that cruzila has proposed 2D tool paths...!
Sorry for the repetition...

[gcode]

We had a Fanuc controlled VTL that was very touchy about arcs

A Fanuc service tech came out and adjusted some parameters that controled the tolerance 

of arc endpoints and radiuses. That solved the problem

[Matthew Hajicek - Singularity]

I've seen this problem on Fadal and Fanuc controls.  Never seen it on Haas.