tool wear ?

How about a stub length 3/16" roughing tool? Gwizard says at the full .250 depth 1220 RPM and 2 IPM there would be .00077" tool deflection which it rates as ok. The tool I based it on is this one:roughing tool
.312 flute length with a stick out of .625.

That would leave .012" for a finishing pass to clean up in the close areas.
 
I'm getting a handle on Fusion 360, I think..., I want to try a deburring pass with a chamfer bit, I've never done that before and these tools have a lot of hand deburring on them. I was thinking of doing the profile cut in 1 pass at full depth but that would make the flipping of the part much more difficult as 6 individual parts over 1 part so I think it would be better to profile 1/2 depth from each side. I'm going to try a roughing tool half depth from each side and then a finishing pass from the final side.

Can I run the chamfer on the first side to deburr then flip it over, finish the profile then do the finish pass and expect a decent finish on the first side chamfer? Or do I need to flip, finish, chamfer then flip it back over to chamfer the first side? that adds another flip into the process.

I want to run the finish from 1 side to eliminate any variance from one side to the other side. maybe fusion will do better in that regard than meshcam did but that remains to be seen.

Any other ideas would be welcome.

Thanks
 
bpimm said:
Ok a bit more info, I had about 1 minute to write the question guess I didn't do very good...

This is the tool I'm making
View attachment 250708
it compresses valve springs 2 at a time, hooks under the cam and the blade goes between the valve shim buckets and the ramp pushes the bucket down and locks on the flat so the shims can be changed.

I make them 6 at a time on a fixture
View attachment 250711
View attachment 250712
Each part is indexed on 2 pins and held down with screws, as it stands I used Alibre to design the part and Meshcam to do the CAM which is fairly limited in how it can set up the tool paths, it cuts the blade section down to finished depth then cuts the outline of the part in 3 passes of .040 each to get to the midline. The part is then flipped and it repeats the process to finish the other side of the blade and cut out. So it makes 6 passes at .040 plus the area of the blade plus it plunges strait down at the beginning of each pass. Mesh cam doesn't do lead in's or ramps just plunges and I know the plunges are not good on the tools.

Tools have been HSS or Carbide they last about the same I use up a tool on each side, if I try to get both sides out of 1 tool it breaks on the second side. I'm running flood coolant 1220 RPM and 4 IPM.

I use GWizard calculator for feeds and speeds.

My original question was would the tool life be better making 4 passes at .060 2 each side at a slower feed rate, I think about 3 IPM will still keep the tool deflection below .001 according to GWizard?

The other possibility I see is that all the plunges are killing the tool and less passes won't make any difference.

I'm in the process of learning Fusion 360 which is much more capable than the Meshcam is and I think I can set it up to plunge into a predrilled hole and eliminate the plunging all together, I just haven't figured out how to do it yet. It would be easy to add a few more holes in the program that pre drills the stock to fit the fixture.

How deep would you guys recommend cutting with a 3/16 endmill per pass?

Thanks
Click to expand...

Do you make these for sale? Looking for one for my 79 Fiat Spider.
If not, do you have a drawing of it that I could use to make one?
 
They're available at Midwest-Bayless. This one is for the 1500 engine in the X 1/9 and 128.
 
You're probably chipping your carbide cutters before you're getting any actual wear. Odds are, it's happening when you plunge. Drilling start holes would be ideal.

I typically use a 1/8 drill-point end mill for edge breaking parts like this. On side 1, mill a channel around the profile for clearance of the edge break tool point. Offset the cutter from the finished profile by .005 to .010" so it cleans up on side 2 to avoid any mis-match between operations. You don't have to do the clearance channel for drill-mills, but I find the finish isn't as great if you just bury the edge break tool. In this case I would use a 1/4" drill mill and, on the same operation, use it to drill all your start holes for side 2.

While you're on side 1, interpolate a nice round pickup hole somewhere to use as your G54 for side 2. Better yet - machine dowel holes for locating on your side 2 fixture - and add a pickup hole on the fixture.

Side 2, go full depth with your 3/16 carbide endmill. Preferably use a stub length - you want shortest end mill that will work. Tool life is better as you're not focusing all the wear in one small section of the cutter (with your current method you're putting four times the wear on just the bottom .060"). The channel from side 1 will provide some relief as well, though it's not necessary for this purpose. Once you get your cutting parameters dialed in, this typically yields better overall cycle time, too.

Start slow and dial up your feed rate until you're happy. With a slotting cut like this your main concern will be clearing chips out of the channel as you go. I'm used to flood coolant, but you could probably rig up a nozzle and use compressed air. Just make sure you set up some sort of shielding so you don't spray chips everywhere.

Hope this helps.
 
You must log in or register to reply here.
Back
Top