Tolerance settings

[rchipper]

Greetings,

 

I am trying to machine a .0235 fillet radius at the intersection of a 150 degree angle but the toolpath will not generate the correct code. I am using a 3/64 diameter endmill (.0469). When I run the simulation I see that the tool generates a small flat move where the radius should be. And the posted code reflects this. I know that some softwares have tolerance settings that allow you to adjust the min/max moves to acommidate things like this. Does Mastercam? I am using X5 and am new to it, I could realy use some help.

 

rchipper

[jeff]

your endmill is .0001 smaller than the fillet, can you use a smaller endmill?

[K2csq7]

Which toolpath?

Look for "Arc filter/tolerance" settings in the operation's parameters tree.

[Brando]

top of screen , settings drop down, pick configuration, then tolerances on left pane, also check total tolerance/arc filter in toolpath params window, not sure which path you are using but like jeff said .0001 smaller rad on tool then the arc you want to cut problably isnt gonna work no matter what you set the tolerance to , but ive never tried that so i really have no idea

[Leigh @ Kodiak]

Greetings,

 

I am trying to machine a .0235 fillet radius at the intersection of a 150 degree angle but the toolpath will not generate the correct code. I am using a 3/64 diameter endmill (.0469). When I run the simulation I see that the tool generates a small flat move where the radius should be. And the posted code reflects this. I know that some softwares have tolerance settings that allow you to adjust the min/max moves to acommidate things like this. Does Mastercam? I am using X5 and am new to it, I could realy use some help.

 

rchipper

 

Settings > Configuration > Tolerances

 

Try changing the minimum arc length

[rchipper]

Wow, thank you. This forum stuff is kinda cool.

 

Well I changed the settings and re simulated and it is doing the same thing. I tried something dif. Instead of trying to generate the radius I removed it and have no fillet. The part dim. calls for a .020 rad. +/-.010. So my thingking is that the tool should follow the geometry and will leave the radius of the tool as a fillet. Well I still keep getting a small linear move at the intersection. ????

 

Much thanks,

rchipper

[rchipper]

Which toolpath?

Look for "Arc filter/tolerance" settings in the operation's parameters tree.

 

I am using contour 2d toolpath.

[Del.]

Have you tried using Optimize to see how it posts out.

[K2csq7]

I am using contour 2d toolpath.

 

Look for the "Arc filter / Tolerance" branch. Put the filter ratio to 1:1 (you may want 2:1 or something different, just make sure it's not "off"), change the tolerances if you want to, make sure the checkbox for "create arcs in X Y" is checked. Also adjust your "min arc radius" on that same page if necessary.

[Guest]

In X6 you "could" go into the internal corner rounding radius and "add" a bit of size to get it to generate a radius move.

 

[rchipper]

Look for the "Arc filter / Tolerance" branch. Put the filter ratio to 1:1 (you may want 2:1 or something different, just make sure it's not "off"), change the tolerances if you want to, make sure the checkbox for "create arcs in X Y" is checked. Also adjust your "min arc radius" on that same page if necessary.

 

You rock. I adjusted the arc filter/tolerance settings and the posted code appears correct.

 

I appreciate your time and effort!

 

rchipper

[rchipper]

Have you tried using Optimize to see how it posts out.

 

I have not. I tried what K2csq7 suggested and the code looks ok. Does X5 have optimization for 2d geometry finish passes?

 

Thank you.

[CJep]

Does X5 have optimization for 2d geometry finish passes?

 

No, that was something that was added in McamX6

[gcode]

Greetings,

 

I am trying to machine a .0235 fillet radius at the intersection of a 150 degree angle but the toolpath will not generate the correct code. I am using a 3/64 diameter endmill (.0469). When I run the simulation I see that the tool generates a small flat move where the radius should be. And the posted code reflects this. I know that some softwares have tolerance settings that allow you to adjust the min/max moves to acommidate things like this. Does Mastercam? I am using X5 and am new to it, I could realy use some help.

 

rchipper

 

 

are you using wear, computer of control comp