Vectric Customer

Good morning all,

Quick question. I do 3D carvings (military items) mostly and have a 5 in tall design that usually takes 3+ hours with default settings in vcarve desktop. I think the default is 50 in/min

bit - 1/32 tapered bull nose

I was thinking about doing a rough pass with a 1/4 or 1/8 ball nose and then running my final pass at 100 mm/sec with the 1/32 bit.

Anyone see any issues with this? Will I see a major difference in quality?

Your shark can cut at 6m/min? (100mm/sec)

You may be able to just double the feedrate without a roughing pass, cutting your time in half. Depends on the material, and machine rigidity.



Quality is going to be directly related to stepover. Feedrate won't make much difference, unless the tool deviates from the toolpath at higher speeds.

Not sure what you mean by default settings in VCarve, there are no such thing when it comes feeds and speeds as they ALWAYS should be adjusted to take account of what your particular machine/material combo is capable of.

With 3D cutting a lot of the movement is in the Z axis which limits how fast the XY can move so often people aren't even getting the speed they've programmed in let alone a faster one.

I am cutting walnut, and when i say default, I just meant what was already input on the particular bit I am using. I didn't have to create to tool choice, it was already in vcarve.

The setting that are "already there" or "default" are just what happens to be there and has absolutely NO rationale behind it.

The values in the stepover, plunge depth, feed, RPM are of no value whatsoever.

The operator/programmer - you - must give values that make sense for Tool Diameter, Machine Rigidity, Material being Cut, Configuration of cutter and anything else that is needed.

Don't rely of the preexisting values.

Leo is absolutely correct. I would, however, like to add that what you enter is not gospel. You won't see much difference between feed rates of 100, 110, or 125 inches/min. Or 15,000, 18,000, or 20,000 RPM. When you are cutting wood, you want a feed rate that is high enough and an RPM that is low enough that you get chips and not dust. This may not be possible with ball nose or V bits, as the different diameter parts will cut differently. (The tip is effectively zero diameter.)

There may be a sweet spot for RPM that reduces the noise.

Small end mills will break with too high a feed rate.

Many machines won't actually move at their maximum feed rate when cutting some projects, the stepper motors can't get them up to speed fast enough before they have to change direction.

If your plunge feed rate is low, any movement that changes the Z will feed at that low speed. For example, a long sloping cut up or down.

Setting Z2 in the material setup to a fairly small value (maybe .06") can speed things up on jobs with a lot of Z movements.

Bottom line: If an experienced operator who is familiar with your machine and the material to be cut has half an hour to fool around, they can probably come pretty close to the best numbers for a new, different project. The rest of us settle for something that works without causing problems. If we have time and the need, we'll tweak a bit to see if it improves things.