Need Help!- How to cut this?

[southernexplore]

It is a simple arch that should be cut in the X-Z axis. I just want to cut it with say a 1/4" EM and step the cut about .150 each cut. Oh yea! I am using V23 Pro.

I have included a small sample of what I am trying to cut.

Thanks,
Tommy

[moldmker]

I took your curve and used Surfaces > Extrude Curve to make it a 1" wide surface.

Then used 3-D Mill > Slice Planar to created the cut.

1. Cut Amount = .150
2. Step Down = .100 to ruf out mat'l (change or eliminate to suit)
3. Lace Angle = 0
4. Arc Fit selected
5. T1 = .25 dia. EM

Attached is the zipped .bbcd
Good luck,
moldmker

edit: I may have misinterpreted your request...did you want just a single arc that stepped down .150 on each pass?

[southernexplore]

That may work, let me try it!!
Thanks
Tommy

[southernexplore]

Yep! Works fine. I even tried to extrude curve .001, used a .25 EM and made a nice .25 wide slot, and even stepped down in defined depth increments.

Thanks Again,
Tommy

[mcphill]

What does selecting "Arc Fit" do in this case?

[moldmker]

Without Arc Fit, the toolpath is broken into many small straight line segments. Creates long G-code file, faceted finish and slow feedrates.

With Arc Fit, the G-code is output as a single G2/G3 arc command per pass, which execute faster and smoother.

moldmker

[mcphill]

Thanks! That makes TOTAL sense now, appreciate your clarification. You then type in the "allowable" deviation from the real model to arc in the "tolerance" box, I assume?

That said, I have not been using arc fit, and doing finish passes at 60 ipm. I don't notice any faceting on a 3D part and the machine hums along without a hiccup in speed. I can totally see where the GCode may be smaller, but not where the machining process itself would go any faster because of arcfit. Could you clarify?

[moldmker]

Originally Posted by mcphill Thanks! That makes TOTAL sense now, appreciate your clarification. You then type in the "allowable" deviation from the real model to arc in the "tolerance" box, I assume? That said, I have not been using arc fit, and doing finish passes at 60 ipm. I don't notice any faceting on a 3D part and the machine hums along without a hiccup in speed. I can totally see where the GCode may be smaller, but not where the machining process itself would go any faster because of arcfit. Could you clarify?

Example, say I'm surfacing the top of a 2" sq. block that has .030" fillets wrapping down to drafted side walls.
The code at that .030" round gets chopped up into small moves that makes my old control (Fanuc 6M) stutter, unless I slow down the feedrate to compensate.
I've run very same code on a late model Haas and it is true that newer machines don't suffer from this.

The most notable faceting is with very large radii (> 6") that can produce .5" long straight segments, no matter what my Tolerance or Facet value is set at.
I check most of my parts under a microscope, that's where it really shows up.

Arc Fit has totally eliminated this for me.

I haven't quite got my head around how the Arc Fit tolerance effects the code. My guess is it's for how it handles splines.

moldmker