Question: Holes in 3D frame not cut out

[hoff]

Disclaimer: this is the first time I'm using v-carve or any cnc-software for that matter, so I might not be explaining myself very well - please let me know if anything is unclear!

Hi folks!

I have an STL file for glasses / spectacles. I import it to v-carve pro 9, set up a 2-sided job, create both sides, and create tool paths for both sides. As you can see from the image I attached, it doesn't "cut through" the holes (within the frame and around it).

When I add more finishing tool paths, it looks like some small sections start to become "zero thick". However, is there a way to set up v-carve so that it 'more eagerly' cuts out the holes, and not slowly reduces them to zero?

Any thoughts on this would be appreciated!

Thanks, Hoff

v-carve screenshot:


stl model:

[garylmast]

In the Profile Toolpath, select Project toolpath onto 3D model.

Gary

[adze_cnc]

Hoff,

Does your material thickness end in an odd number (e.g. 0.375 inch)? If so, I expect "rounding errors" in the software when dividing by 2 (double-sided).

VCarve seems to have problems with doing math when an odd number is in the thousandths position of the decimal.

For example if I specify the thickness of material to be: 0.711 inches and I do a profile pass that has a starting depth of: 0.125 inches and a cutting depth of: t-0.125 (that is the thickness variable less the 1/8" start depth) VCarve will generally warn me that my cutting depth exceeds my material thickness. Even though t-0.125+0.125 should be equal to t

Steven

[FixitMike]

If you use the profile toolpath, be sure to add a couple of tabs so the center doesn't come loose and damage another part of the model. Also, set the start depth to a value approximately equal to the highest point of the area to be cut. You can get this height by placing your cursor on the highest point of the lens in the 3D preview and reading the value at the bottom of your window. You may also want to use a straight bit instead of the ball nose used for 3D. Run the profile toolpath after the 3d cuts.

If you don't want to have tabs left with a piece to remove, you can also use the Pocket tool path in a similar manner. It will take a little longer than the profile toolpath, but the area will be completely cut out.

If you don't want the finishing toolpath to spend time on the lens area, draw a vector that is inside the lens boundary by just a little more than half the ball nose radius, and another that the same amount outside the entire cut area and select those along with the STL for the 3D toolpaths. In your 3D finish toolpath, check the Machining Limit Boundary as Selected Vector(s). Note that the vectors define the limit of travel of the center of the tool. The vector for a pocket or profile will be offset from the machining limit boundary vector.

Another option is to use the same tool for the profile or pocket cut as you use for the 3D roughing toolpath, and save its toolpath with the roughing 3D toolpath to eliminate an extra tool change. Or, if you are using a finish cut only, you can use the same ballnose with a profile or pocket cut, but if the ballnose has a taper, be sure the lens outline vector is slightly smaller so the taper doesn't touch the area alongside the cut.

Check the preview carefully, it will accurately show what you will be getting.

[FixitMike]

Another thought: If this is a 2 sided job cut wilth a ballnose, the lens cutout surface will have small waves in it from the ball nose radiius. The actual surface will only cut through at the very tip of the tool. This may be what is preventing the preview from showing an opening. Also, the ball nose radius will leave a small ridge around the inside of the lens opening in the actual part.

[hoff]

[quote="garylmast"]In the Profile Toolpath, select Project toolpath onto 3D model.

Thanks garylmast, when I use a profile toolpath with 'project toolpath onto 3D model' selected, I get this, still not right...



I think I'll try to mill the piece anyway and see what happens. If anybody has any other suggestions, I'd be happy to hear them:)

Thanks for lot FixitMike for you advice!