Poor surface Finish

[KMartin]

Hi Everyone - Can I please get some help with this tool path . I'am getting a poor surface

finish using this type of tool path . The Machine I'm using is a Hass VF1 . There is no problem with

the tool .... checked the run out . I'm limited to a 1 meg program because of floppy .( converting to DNC soon )

I would like to us Raster but programs to large . I just don't no if it's my settings in Mastercam or

setting in machine .I'm getting a very choppy finish . Thanks for any help .

The file is ... ftp://ftp.mastercam-cadcam.com/Mastercam_forum/X6_FIles/test1

 

 

MCX6 MU3

[htm01]

check setting 85 corner rounding, factory set to .025

[duckdogers]

we had this problem when we first got our hass.We run our filter settings high which makes program long.We had to go to dnc because of the size of the program and the restrictions of either the floppy or the machine control itself.

[Machineguy]

More info would help us.

What year machine? IS high speed machining turned on in the machine?

This topic for filter settings for a Haas was covered just a few weeks ago. Do a quick search. Haas, Filter settings.

 

 

Machineguy

[KMartin]

The Hass machine is 15 years old and we are not using G 187 .

The corner rounding is set at .025 . Thanks for the help .

[Oscar R.]

I took a look at your toolpath there. Looks like you have it going across the surface.

I would turn the machine angle 90 degrees in either direction if your conditions allow.

This will generate less code for you and let the tool do a better job on your finish.

[htm01]

run the program at different 85 settings and you'll see the difference. we were running the same job in 2 machines and one was reset by the has tech to .025 and the other is set to .005

[Allan]

I noticed that you are not using the arc filter, I've uploaded the file with the arc filter turned on test1_ab.mcx-6

 

Their have been issues with the arc filtering on Haas machines but since this is just a half round circular channel I would think you should get decent results.

 

 

Allan

[KMartin]

Thanks Allan - I'll start with those settings .

[Thee Rickster ™]

I use hass also

 

Very common path and surface type here, working on something now.

(although I use flowline....)

 

Change the cut angle to 90, doesent look necessary to sweep the arc

IMO

 

 

 

 

 

Cheers Rick

[MrFish]

The HAAS will struggle to keep up with that feed rate even with Highspeed machining turned on. I wouldn't feed at more than about 120 inch/min if you want to achieve an accurate part.

[Thee Rickster ™]

The HAAS will struggle to keep up with that feed rate even with Highspeed machining turned on. I wouldn't feed at more than about 120 inch/min if you want to achieve an accurate part.

 

hmmmm, My hass high speed mills run at 200plus all day everyday with great accuracy.

my older vf6, bare bones only runs a max 120ipm because of the corner rounding issue.

[KMartin]

Changed the cut to 90 and got a much better finish . Thanks Rickster .

[htm01]

hmmmm, My hass high speed mills run at 200plus all day everyday with great accuracy.

my older vf6, bare bones only runs a max 120ipm because of the corner rounding issue.

the has ss uses a 12 mm pitch ball screw, the vf a 8mm and the vm a 6mm, we traded in our ss for a vm because it would not follow our mold surfaces