Surface Rough Cutting Air

[Mic6]

I'm trying to rough some large chamfers with rough parallel. How can I make the tool start below Z0. I'm leaving .05 on the drives. The tool cuts air at Z.05, then finally starts to cut. My max stepdown is .250. TIA

[gms1]

Try using the depth cuts "Adjustment to top cut" to force it into the material on first cut. If incremental doesn't work, you could always use absolute depths.

[strabe]

What toolpath are you using? Certain paths have a depth cut adjustment that can eliminate the air cuts.

[strabe]

I see it now. gms1 is right. That will change your starting depth.

[Mike S @ S4A]

surface rough parallel employs "cut depths" on tab three; if they'e expressed as absolute they're true absolute elevations in the current toolplane. If they're expressed as incremental then they're incremental from the drive geometry's range of elevations

[Mike S @ S4A]

Here's a snippet from our advanced mill training manual (which paraphrases what you'll find in the Mastercam help file:

 

Essential Concepts -

Depth Limits & Cut Depths

Depth limits and Cut depths specify the range

of Z elevations to execute cuts within

for surface toolpaths.

Depth Limits are literal. Cuts occur only between

the minimum and maximum specified.

Cut Depths settings are a bit more involved.

Absolute cut depths are just like depth limits.

All cuts in the toolpath are equally spaced between

the minimum and maximum limits.

Incremental cut depths* are measured between the

top and bottom of the part. You can enter an

adjustment amount to the top and bottom cuts.

Mastercam automatically calculates the Stock to

leave on drive surfaces parameter into the cut

depths, and spaces cut depths equally.

* Used for most rough surface toolpaths and for finish contour toolpaths

If the depth limits remove sections of the toolpath

gap settings will determine the tool motion between

the remaining sections. Gap settings might require

movements that conflict with the depth limits.

In such cases, the gap settings take precedence.

[Mic6]

Thanks. So I adjusted the top cut and it worked fine. I changed tools to a 2" face mill. Would I be better off not using a surface rough? I want to step down .15 at a time, stepping down to follow the chamfer angle. Kellering is the name? The .750 tool I was using just passes over the already cut surface twice. There's more non-cutting than cutting!

[Mike S @ S4A]

Just be careful with a tool literally defined in mastercam as a facemill; stepovers are based on effective cut diameter, not outside body diameter...forgive the redundancy if you already knew that.

[Mic6]

Thanks Mike, I just used the .75 em and cut the dang air. I'll look into this more next time.

[Rstewart]

You need to be using Rest Roughing from a STL. Very little air cutting time!

[Nils N]

Rstewart, could you expand on that a bit. I've had some of the same problems with new stock shapes that are stair stepped shapes. I've had a bit of luck using a trimmed tool path but I can only trim it one way ( as in the length) so i still cut air in the width. Can you use the rest rough STL with the original stock shape?

[Rstewart]

I would have to go look up some of the parameters im using, but there is still SOME air cutting time.

Using STL rest rough is still much better and a whole lot faster than just a plan ole' Roughing TP.

I've found that if your rest tool isn't smaller than your rough tool you get more air cutting time too. I'm no surface toolpath genius, so I'm sure someone else can help alittle moe

[Tony35]

quote:

---

Would I be better off not using a surface rough? I want to step down .15 at a time, stepping down to follow the chamfer angle.

---

not sure what your chamfer looks like but you could use depth cuts and turn on taper angle to rough out the chamfer at .15 per cut