DOC ? 2 schools of thought..

[Fred @ Slate Industries]

Hi Folk's

I have been taking light and fast cut's forever (.500 single flute w/.030 r)

5000 rpm at 30.00 ipm / in P-20

The other Programmer take's way deeper cut's at a slower speed and feed.

He also doesn't Pilot drill anything under 1", "Your only using 1/8th of the entire bottom edge of the drill bit your way"

 

 

What's you theory?

[uncle_dolan]

pilot drilling is only necessary for larger diameter drills with thick webbing. For normal HSS drilling bits I would say you would need to pilot drill from 0.75 upward to be safe. For carbide drills and modular drills this is not the case. When I'm machining Aluminium I like the small cut depth and high feed approach, but for steel alloys i prefer to take deeper cuts...especially with chatter free cutters...they are made for it!

[BenK]

I take a deep depth of cut but a light radial depth and apply chip thinning. You can really remove material fast. I have a 1045 job that I'm going to be cutting 1.6" deep at 10% radial step over with a .625 EM at 4200rpm and 200ipm doing it this way.

[Chris Rizzo]

challenge him to a head-to-head. Same part. Tools of each's choice. Cut time and tool wear will be the judge. Check out some numbers in my dynamic milling database and you should smoke him.

[Guest CNC Apps Guy 1]

I used to be a light DOC fan... since changed my mind after running some tests. For raw MRR... Tool's LOC and frmo 5%-15% stepover, you'll smoke the light DOC on days that end with "y".

[Glenn Bouman]

Using the Opti-Rough and Dynamic toolpaths you should be able to go 3X dia for depth of cut and 5% to 10% stepover at higher feedrates.

 

You will benefit by quicker cycle times, better tool life (Full flute utilization) and less cutting pressure (less vibration on light duty machines)

Smaller tools can be used:

Less carbide, less expensive

Fewer tools can be used

 

 

Here are examples.

 

[Goldorak]

Using the Opti-Rough and Dynamic toolpaths you should be able to go 3X dia for depth of cut and 5% to 10% stepover at higher feedrates.

 

You will benefit by quicker cycle times, better tool life (Full flute utilization) and less cutting pressure (less vibration on light duty machines)

Smaller tools can be used:

Less carbide, less expensive

Fewer tools can be used

 

 

Here are examples.

 

 

 

+ you don't have to hold your part down with 50 clamps and 2 vises, dynamic toolpath don't need excessive force to hold the part

 

this can save many hours of production at the end just in setup and part changing time

[overthecrossbar]

For Aluminum with high speed dynamic I go 1.5 xd and 15%-25% stepovers at max rpm, chip load depends on tool dia.

[Teh Bear without Brains kinda idiot]

For Aluminum with high speed dynamic I go 1.5 xd and 15%-25% stepovers at max rpm, chip load depends on tool dia.

~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

I got to doc 2,5 dia and will try this week 4 dia

Spindle load is constant and small ,chip extraction is great and work is done much faster than usual

Microlift is cool feature .

Great stuff

[Newbeeee™]

You'll also get a better part. Less cutting forces so less distortion on thin wall parts.

[RaiderX]

yep am changing my aproach and methods dramaticly on this. used to be a fan of lots of shallow cuts. no more of that cycle eating beast for me except under certain conditions that require it. think of the tool wear on just the end of the end mill. dynamic tool paths rock.

[Guyinthedesert]

It also depends on what your part looks like. Some parts we do have a lot of detail, such as valve bodies with ports comming off at all angles. Using a DOC of .100, you can rough out much more material.

[Teh Bear without Brains kinda idiot]

It also depends on what your part looks like. Some parts we do have a lot of detail, such as valve bodies with ports comming off at all angles. Using a DOC of .100, you can rough out much more material.

~~~~~~~~~~~~~~~~~~~~~~~

In such a case you need to use

 

OptiRough toolpaths

The 3D surface high speed OptiRough toolpath supports cutters capable of machining very large depths of cut. It uses an aggressive, fast, intelligent roughing algorithm based on Mastercam’s 2D high speed dynamic milling motion.

 

 

 

A single OptiRough toolpath can cut material in two directions, on step downs (-Z) and step ups (+Z). This highly efficient bi-directional cutting strategy removes the maximum amount of material with the minimum of step downs, significantly reducing cycle times.

 

As step downs are calculated, the dynamic roughing motion clears the material in the -Z direction, avoiding any islands.

 

If you activate step up cuts in the toolpath's Cut Parameters, Mastercam calculates additional slices in the +Z direction to remove any material left behind between the step downs—for example, islands or large scallops on angled walls. The step up cuts use a 2D high speed dynamic rest motion to clear leftover material. Step up cuts are ordered between step downs.

[Guyinthedesert]

I'll have to give Opti-rough another look. I never rally used it because of the enormous file size it creates.

[Glenn Bouman]

I'll have to give Opti-rough another look. I never rally used it because of the enormous file size it creates.

 

 

 

Turn on the arc filter, I am not sure why it is defaulted off. I have found the file size to be smaller as 3X dia in depth with a .05 cut width generates less code than .05 depth and 75% Dia of cutter stepover.

[Guest CNC Apps Guy 1]

Yeah, the bottom up approach works awesome. Perfect for valve bodies with protruding stems.