depth on flowline with a bullnose

[Tim Pruett]

Is there anyway possible to get a bullnose endmill to cut to the proper depth. I'm cutting drafted walls of .5 to 2 degrees. The end mill is a .375 garr with .o2 corner rad. I give it the max depth in the cut depths section but it won't go the the depth I want.

[mkd]

well, by how much is it missing the depth? .020"? .500"?

how much stock r u leaving on check surfaces?

 

1/2 degree is not much. sure there is no negative draft?

 

pictures?

[strabe]

I use flowline a lot and never had a problem. Maybe try a different toolpath. Parallel perhaps?

[jeff]

Are you SURE that your surface is drawn to the depth that you want to mill to?

Never had a depth problem with bullnose/flowline,and I never use the cut depths parameters.

[kens1]

Is tip control set to tip or center?

[Tim Pruett]

The surface is not negative draft.

The tip control is set to tip.

I extended the surface .1 past where I want to mill to. Its kinda like surface finish contour when it won't cut the last .006 if you're steping down .01. In this case I'm stepping down .01 and it's missing the depth by around .005 or so.

[jeff]

is the corner where the wall and floor meet sharp? or have a radius smaller than the tool?

[Toonz]

Do you have a value set in the "Stock to leave on drive" ?

[Oppiz]

Have you made sure that your depth limits is setup properly?

[Tim Pruett]

Im only cutting one surface there is no floor.

Stock to leave is set at zero.

I have no check surfaces.

Tip control is set to tip.

As far as I know the depth limits are set properly. I have them set to -.02 and -.503. I would like for it to cut to -.503 but the last cut is at -.4993 on the toolpath i'm looking at right now. Im sure I just don't have something set correctly. I don't use flowline very often. I might add that I'm going back in with a flat bottom endmill and cleaning up the corners and it's going exactly to the correct depth every time without any problems. That's what got me thinking that it had to be the bullnose giving me the problem. They are the same toolpaths just copied and a differen't endmill being used.

[Colin Gilchrist]

Is your filter turned on? Try turning it off and setting your tolerance to .0001.

[Colin Gilchrist]

Also, try changing your step over to .009, sometimes a little tiny parameter change can get things to work...

 

The other recommendation I have is to try running ram saver. I've had toolpaths that would calculate the same, even when I changed parameters. For example, I'd adjust the cut depths and no change would happen. Then I'd run ram saver, or restart mastercam and the parameters would start working again...

[mchin-pilot]

Flowline is the most "touch of a button type toolpath". Things dont go wrong with that.

 

Just keep trying some different values/settings

[Tim Pruett]

I tried turning off cut control, setting the cut tolerance to .0001, running ram saver and messing with the stepover amount. Nothing worked except for changing the stepover amount. I changed it to .009 and it got closer to the depth I wanted but it was still .002 or so away. So I started changing it in .0001 increments both less and more than .009 and never could get it any better.

I read the help section under cut tolerance and it said something about turning on a 3d advanced tool refinement feature using the mastercam applet. I'll try to figure that out and see if that makes a difference.

[gcode]

Do you have it set to tip comp or center comp.

Some earlier versions (X3??) defaulted to "center comp" which caused all sorts of trouble.

A possible workaround.

Create a flat plane at desired Z depth

and call it a check surface..

set your min/max depth well below the check surface

 

[ 06-11-2010, 07:51 AM: Message edited by: gcode ]

[Tim Pruett]

Ok, I turned on the 3d refinement feature and that seemed to help on the drafted surfaces that i'm stepping down .009 on, but i'm also cutting some non drafted surfaces stepping down .025 at a time and they are still coming up .016 shy of the depth I want to cut to. I tried extending the surface and that didn't help I also tried gcodes' suggestion about using check surfs and making the max depth well below where I want to cut to and still come up a couple shy of the depth I want. I also tried cutting from the bottom up but it still comes up short of the depth. I guess it doesn't really matter in this case cause i'm squaring up the corners with a flat bottom endmill but I may want to just use a bullnose to finish with sometime and I would like to figure this out now. I really appreciate all of the input. I don't know where I would be if I didn't have this forum and all the help. I'm really the only one at my shop running mastercam.

 

I'm running X4 mill lvl 3

[jeff]

Try putting the file on the FTP so that we can better help figure out the problem.

[Tim Pruett]

When I try to get on the FTP it says I have to hit the page button and then hit open in windows explorer and when I do that i have to put in user name and password and it won't let me log on. Should this username and password be the same as my forum username and password? Also do i have to zip the file to copy it to the FTP?

[Guest]

login: mastercam

p/w: swiss

[Tim Pruett]

Thanks John.

Ok I copied the file in the X4 files folder named flowlinedepth. I made a new slimlined version of my file by copying one cavity block and then creating two toolpaths on it just like I was using in the main file but they actually cut alot closer. The first program only came up .0005 shy of the depth and second one only came up .0047 shy.

[Steve Z]

Tim, when you posted the operations. Did the depths match what you stated is short for your depths?

[Tim Pruett]

I just posted one off of the simplified file and the depths match on it.

[Elmer Fudd]

Try turning off the depth limits and selecting the floor as a check surface.

[Tim Pruett]

Ranger Dan, I tried that and told it to leave .002 on the check surf and it stayed away from it buy around .01. I had the surface that I'm cutting extended buy about .05 originally and when I tried the check surface method without the depth cuts turned on it cut right through the check surface(floor).

[Steve Z]

I think if you try and extend or redraw your surf to a even number you can divide into, that may work. Right now your actual depth of cut for operation #2 is 1.4534". Try making your surface 1.46" long for your DOC. Then make your stepover distance 0.02". That'll be 73 even passes. Haven't proven it out, but try that.