Bit Stepover percentage

[jTr]

Seems simple enough, but am looking for a clearer understanding of the Step Over value in Partworks. When cutting pockets (such as dados), Is this the amount the bit advances past first cut, thereby removing more material, or is this the amount of bit hanging over in the previous cut path?

Would like advice on an optimal percentage for this procedure - current default on .25" bit is 30% (.075 or just over 1/16th). Trying to improve cycle time for machining this type of joinery by increasing to 60-80%, if I understand this value correctly. Hoping I'm not out of line asking a .25 bit to remove .20" material as it spirals out to pocket those rabbets and dados...

Thanks!

jeff

[gc3]

http://www.vectric.com/forum/viewtopic.php?f=2&t=12881

[feinddj]

Stepover is the percentage of the bit diameter for the next pass after the entry into the material. Offset is the amount of give from the vector that you selected. Say you select a square with no offset (0.0), the path will cut right to the square. With an offset of .125, it will cut an eighth in. make the offset negative and it will over cut. Useful for compensating for bit diameters or making the hole just a little oversized without redrawing.

Hope that helps.

David

[jTr]

I will proceed to bumping that step over percentage up to 80%, since depth of cut is only .25

Running 9660Alpha for over a year now, and beginning to look more in depth at "tweaking" and paying closer attention to those defaults. Love this machine, but still feel awfully green at times...

Thanks for the help!

Jeff

[Brady Watson]

For all 2D operations, set stepover to be 40% and leave it. Only when cutting very dense material such as aluminum or rigid plastic would I reduce it to less than that value to minimize shock loads when the bit steps over into the material. More than 40% SO will leave material in areas that should be cleared. (Little triangular pieces)

For 3D finishing operations using a ball end mill, you want to run 8 to 12% the tool diameter to get a good finish. Less than 7% and the law of diminishing return comes into play. You can run 15-20% if you want to do a coarse 3D finish on large reliefs without a lot of detail, where a few passes with a sander smooths it all out.

-B

[bleeth]

You can also take into account what material you are cutting. Soft material like sign foam or mdf can take a larger stepover. So for a pocket 1/2" deep in sgnfoam with a 1/4 or larger end mill I would likely go 85% just as I do when shaving my spoilboard 1/16-1/8.

Oak, maple, etc it pays to be more gentle (40%) or so. As you gain experience you will get a feeling for how much you can push the limits without screwing up and even when to go a little easier as a bit has had more use or is even a higher or lower quality bit.

Technically it is a science but in practice it is artisan! As you do more your learned instincts will help. In the beginning you may screw up some parts or bits but this is all part of the learning process like skinned knees and elbows when learning to ride a bike or that well remembered feeling from holding a nail wrong!

It goes along with listening to your cutting-If it's screaming and your cutting wood you have your feed/speed balance wrong. One sound can mean too aggresive and another not aggresive enough.

[jTr]

Brady and Dave,
- I was hoping someone would clarify where not to step as I begin "tweaking". Hate to question every default, but do realize I need to hone things to my methodology for maximum quality/productivity.

Thanks again!

jeff

[Brady Watson]

If the doorbell rings & there is a brown bag on fire, do NOT step on that! :D

There is precisely ZERO logic in ANY of the default settings in ANY tool database. Start with 40% for 2D work, 10% for 3D work. Step down will vary with material and bit. Experience will tell you what the other settings are. Start slow & conservative, then feather in more speed or depth as the tool & machine allow. If you listen to the machine, it will tell you what it wants in order to get to the sweet spot.

-B

[bleeth]

What he said.

[myxpykalix]

If the doorbell rings & there is a brown bag on fire, do NOT step on that!

...now you tell me...:mad:

[feinddj]

Jeff,

The answer is "it depends." Every situation is different. Once you hit the sweet spot for the bit and the material that's where you should be. Overfeeding the bit can cause heat buildup and dull the bit prematurely. Underfeeding can causes breaking, bad cuts and might damage your router if it doesn't snap the bit first. Sometimes you have to trade a longer time to do a pocket with a smaller bit because you can cut the rest of the job with that same bit and not change it.


David