simple surfacing question...

[TurboME]

Well I think it should be simple. I'm trying to cut the concave surface in the part show in the attached picture.

I'd like to have the tool plunge outside of the stock, outlined in red but I can't figure out how.

It seems like a flowline routine would be the best method but all of the entry moves are plunges into the part.

Is this possible?

[100]

Create a new surface that matches the contoured surface you have but extends beyond the red outline and cut that. You will cut some air but this is a simple method.

[LUNCH TIME]

try creating a rectangle where the bounding box is and use as boundry for work. then surface rough pocket, in the ramp entry box check "plunge outside of boundry"

[trls63]

Originally Posted by TurboME Well I think it should be simple. I'm trying to cut the concave surface in the part show in the attached picture. I'd like to have the tool plunge outside of the stock, outlined in red but I can't figure out how. It seems like a flowline routine would be the best method but all of the entry moves are plunges into the part. Is this possible?

finishing or roughing? cause for the roughing you can do just like LUNCH TIME said and draw a rectangular boundary , select a rough surface pocket toolpath and chk the option Plunge outside boundary

[LUNCH TIME]

depending on your rough tool dia, you will need to use rest mill cut to reduce the stock for finishing. maybe a parallel pass would work as well,just have to see how much material is left!! diameter matters in this case as well as step down.see which produces the "safest" method.nobody like broken cutters!!!! i like scallop pass for finishing of surfaces myself. happy chipp'n

[wholepair]

What is it?

It looks like something you would use to clamp on a cylinder/tube...

How big is this part? What is it made out of? Is it half of an assembly? Is the concave surface defined by real circle geometry?

If the concave surface is a true circle I would suggest doing it in another operation with just a side cutting arc interpolation, or even a boring tool. You will save time and get a better finish. Not that you can't get a good finish with surface toolpaths, but it usually just takes a longer time. If you are making two of them you could do both parts at once and then cut them in half and lastly machine the outer profile. I don't know enough about your part, but these are my thoughts.

[cadcam]

I would cut uesing surface rough pocket with a bull end mill. due the main profile as a simple contour the go back and copy the center surface and then use create surface untrim to make is a singal surface without the holes.

then do a simple flowline pathe to finish.
What is the Material?

about 15 to 20 mins worth of work. Hope all goes well.

[jcwebb]

Use a flowline surface toolpath. Then go under "gap settings" and add half the diameter of the tool to "tangential line length".
That's it.

[jcwebb]

Or extend the existing surface out half the diameter. then flowline.
Use ball endmill with .005 stepover and your finish will be good looking.

[cadcam]

Why are we telling him to extend or "tangential line length". Half the tool.
I could see using the "tangential line length" and going say .02 more past the edge.

but if we are talking about not plunging in to the surfce then you the Direct option to get the tool in at an Angle away from the surface.

[jcwebb]

It all depends on how deep the surface cut will be.
Half the diameter over will ensure that the tool doesn't plunge into the material.
If just skimming the surface after roughing it, then sure only .002 will work.