Follow Us
Popular posts
- What If Dyson Made CNC Routers Instead of Vacuum Cleaners?
- CNC 4th Axis Basics: Routers and Woodworking
- 10 Tips for CNC Router Aluminum Cutting Success
- MIT Students Create Hand-Held CNC Router: You Gotta See This!
- Tale of Two Engines: Giant Crankshaft and World’s Smallest V12
- CNC 4th Axis Basics: Workholding
- Desktop Manufacturing is Here With Two Amazing Announcements
- Several Customer-Driven Updates to G-Wizard Editor This Week
- Turn Toolboxes Into Workbenches
- Making Cell Phone Cases With Syil, Fadal, and G-Wizard
Recent Comments
- Paul Mc on An Entire 3D Printed City?
- dbtoutfit on Nesting Software from Sigma Tek to MyNesting.com: An Introduction
- Take the CNCCookbook 2013 CAD Package Survey - CNCCookbook CNC Blog CNCCookbook CNC Blog on Results from the 2012 CNCCookbook CAM Software Market Share Survey
- Take the CNCCookbook 2013 CAD Package Survey - CNCCookbook CNC Blog CNCCookbook CNC Blog on Results from the 2012 CNCCookbook CAM Software Market Share Survey
- Jamie Fritz on What If Dyson Made CNC Routers Instead of Vacuum Cleaners?
Categories
- 3D Printing (22)
- Beginner (88)
- Blog (593)
- Business (55)
- CNC Projects (118)
- CNC Router (28)
- Cool (139)
- FeedsSpeeds (47)
- GCode (51)
- Guest-Post (10)
- Manual (8)
- Products (49)
- Software (177)
- Techniques (219)
Thinking About High Speed Machining, Corners, and Stepover
I recently got a note from a G-Wizard customer who was interested in understanding some tool wear issues he was seeing. He had two toolpaths, one an HSM (High Speed Machining) toolpath and one a conventional toolpath. He was cutting hot rolled steel with a 1/2″ stub length carbide endmill, and making lots of small pockets just over 1/2″ deep. The scale on hot rolled can be tough on cutters, so he made a pass to remove that first. His question was all about tool life after that pass which was made with a different cutter.
The HSM cut was made by pre-drilling an entry and then running 2800 rpm, 0.005″ chipload, and stepping down 0.185″ per step. Stepover was 65%. The conventional cut was made by contour ramping entry and constant stepover of 0.045 and a much higher chipload of 0.014″ and higher rpm of 4500 rpm. Tool life was far better on the conventional, so his question was basically, “Why didn’t the miracle HSM toolpath do better?”
This is a very interesting case because it really gets into the nuts and bolts of what the advantages of HSM toolpaths are versus conventional toolpaths. Here was my answer back to him:
It’s all about the stepover or radial engagement.
On the high speed version, you’re running 65% stepover. On the non-HSM version, you’re running 0.045 / 0.500 = 9% stepover.
So two things to consider.
First, the only difference between an HSM and a non-HSM toolpath is the HSM plays tricks to avoid radically increasing the engagement of the cutter in corners. For square corners, and 50% stepover, you go from 90 degree engagement to 180 degree in the corner, so the cutter works 2x as hard in the corner. So, the HSM path doesn’t have to work as hard in corners as your ramping path, but there’s no other special advantage it has as a result of the HSM paath.
That brings me to my second point.
With G-Wizard, we can convert stepovers to tool engagement angles. So, the 65% stepover, if we key all that in, turns out to be 107 degrees. It’s a little better than the 180 degree case, but not hugely.
G-Wizard’s Tool Engagement Angle Calculator
If the 9% stepover were done with an HSM toolpath, it would be a 34 degree engagement–which is really starting to cook with fire.
The reason this engagement angle matters so much is due to two factors: chip clearance and the ability of the tool to cool. It’s pretty easy to see, once we start thinking of these angles, why they matter. If the tool’s flutes are shrouded only 34 degrees out of 360 of a full rotation, they’re pretty wide open. It’s easy to get the chips out of the way and the flutes have a lot of time in air and coolant to chill down during the revolution. With 107 degrees, there is a lot less time. We go from only cutting about 9% of a rotation to 30%. The cutter is working at least 3x harder.
So let’s put all this together. If we were only cutting in a straight line, every toolpath would be an HSM path–no corners to worry about. And, of the two cuts you used, the 0.045″ stepover cut is 3x easier on the cutter. All other things being equal, it can go 3x as fast in feedrate or it can have 3x the tool life at same speed, etc.. Those are over simplifications, but you get the idea.
In this case, the stepover on the HSM path, was so close to a non-HSM in a square cornered pocket (e.g. 107 degrees engagement vs 180 degrees) that you didn’t get a lot of benefit from the HSM path.
FWIW, a good starting stepover to try for HSM is 15%.
