I recently finished the Building Block Series and am trying my hand at milling a turners cube. I milled the first face using the 3D Adaptive clearing followed by contour tool paths. I ran the 3D adaptive and noticed some slightly unpredictable patterns (see Turners Square RJS). As I machine each success face, there will be less material and I will be more delicate to hold in the vise.
For subsequent faces, I plan on using a 2D contour tool path and forget the 3D adaptive. I feel this give me more control over the exact tool path, lead-in, lead-out etc. (see Turners Square RJS Contour Tool path).
Here are a few questions:
Should I use a 3/8" endmill to bore the smallest hole in the center which is 17/32 to give more space for lead-in, lead-out?
My speeds/Feeds calculator (CNC Cookbook) suggest feed rate of about 16 inch/min for roughing but about 80 inches/minute for the finishing pass. Fusion gives a warning that the finishing feed rate is higher than the roughing. Any thoughts on this one?
Also, if you have any ideas as to how to make these tool paths give the least chance of pulling the part out of the jaw… Please let me know.
I had my students, drill hole 1/2" drill, then 2D Contour with a finish pass on both Z and contour for each 3 levels and a simple 2D contour on 17/32 hole (near zero leadin and leadout. We clamped holding 1/8 of part each time. (We had finished machined the cube faces in a different process. Later we machined this on our 5-axis machine in 2 setups.
Thanks for your reply, Stephen. When I changed my plans, if I understand you correctly, that is what I did with the file linked "Turners Square RJS (Contour Toolpath). Can you explain what you mean by “We clamped holding 1/8 of part each time”. Does this mean you used parallels and only held the part by 1/8 of an inch? If so, why would you do this as opposed to holding the whole part deep in the vise?
In G-Wizard Feed & Speed, slide your “tortoise - hare” to 29%, which should reduce your finish cut’s feed rate…
clamping the cube deep in the vise may slightly distort the area you’d be milling. you could check this by setting a dial test indicator on an inside rear surface, then watch if it moves as you tighten the vise.
Most of our setups we only clamp on .090" of material. Our end stop and parallels are suited for top hat machining, if possible we machine 5 sides in 1st op and then 2nd op we remove the remnant. I did have one student that used a 2" long endmill and machined the square sides and faced top and machined counterbores in 1st op, 2nd Op flipped the part removed the remnant and machined the 2nd multi counterbore, then 3rd - 7th ops were just repeats of the counterbore op…
Sorry I missed your post. I am running a small 2HP benchtop mill. I intentionally used the G-Wizard set to like 5 or 7 percent because I was trying to take very light cuts since at some point there will be very little material left to hold on to. The max rpm on this mill is only 3200 so I guess I am trying to take gentle passes. Does this make sense?
I understand, however be sure not to take it too easy … watch your chip load / thickness - the tool must take a cut and not rub.
If you haven’t already done so, set your machine’s rpm and power limits in G-Wizard (settings, advanced)
If you’re concerned the work piece may be ripped out of the vise, this link may help:
Also, you can do some math to calculate the cutting force: G-Wizard will provide the torque needed to make the cut (be sure to select the correct material, e,g, 6061-T6, etc). Divide the torque by the endmill radius to get the tangential force. convert this to lbs. Since the cut usually occurs above the top of the vise, multiply the tangent force by the leverage ratio (distance from top of vise to top of cut). Add a 25%+ “safety factor”.(Note: dull tools , rubbing, or chatter will increase the force.) Compare this to the lb force the vise is applying to the contact area (sq-in) on the work piece. (this assumes clean dry part & vise surfaces. With coolant or cutting oil, you want to significantly increase the force required to hold the part / compensate for less “jaw friction” - Divide the cutting force by 0.2 to ).
This isn’t exact, but it will get you very close. Here are a couple more useful links: https://www.kennametal.com/us/en/resources/engineering-calculators/end-milling/force-torque-and-power.html Give tangential cutting force in lbs. Bolt Torque, Axial Clamp Force, Bolt Diameter Calculator plug in your mill vise’s screw data (and use a toque wrench to tighten) to determine clamping force.)
Cheers
