Lathe roughing

[Thad]

We had a lathe demo by our reseller yesterday and will soon be getting a 30 day trial. I put a file in the MCX2 Files folder called CHUCK2.MCX. I'd like some advice on roughing the red surfaces. Using the lathe rough toolpath, is there a way to ramp into the stock? The lead in/out allows for an angular approach, but to get to the cut depth, the tool plunges straight into the material. I'm not a lathe guy, so to put it in mill terms, I'd like a tangent line then arc into the cut, like the lead in/out options in a contour toolpath. The tool that we use doesn't take plunging too well.

 

For those that can't get to the FTP...

.

.

 

Thad

[Goldorak]

plunge toolpath and set your tool at 90 deg

 

and use a face groove

 

[Colin Gilchrist]

Axela is on the right track.

 

Thad, for something like this I would call a couple tooling suppliers and get their recommendation on a new holder and insert to do face grooving. For Lathe work like this you would normally do some type of plunge entry. Ramping into the stock is going to put more wear on one corner of your insert and the insert won't last very long. Since you mentioned that your current tools don't like to plunge, I thought I'd suggest looking at a different cutting tool...

 

HTH,

 

 

P.S., I'm more of a mill guy too, I'll defer to the experts on this one...

[Columbo™]

+1 on Goldorak

 

A face groove tool is the way to go for this application. Also ramping would add eccesive wear onto the tool. I would, on the finish pass break the edges by generating a small radius like the picture above.....good luck Thad

 

[Thad]

Despite causing excessive wear on the tool, is ramping even an option? My dealer couldn't find a way to do it. It would come in handy with other tools/situations.

 

Would anyone be willing to program the part and put it back on the FTP so I can see your selection of toolpaths? We ended up putting it on the mill to cut the red pocket.

 

Thank you all for your input. I welcome any further comments.

 

Thad

[rdkllkng]

If you had live tooling on your lathe you could endmill it out if you are more comfortable with milling.

 

ditto:

+1 on Goldorak

+1 on Columbo

[Goldorak]

Thad , roughing + finish on a mill is the best way

at the same time you can drill the 3 holes

 

i checked the file on the FTP and the "nipple" is a bit too small (1.25dia x 1.75dp ) for a face groove

[Thad]

quote:

---

If you had live tooling on your lathe you could endmill it out if you are more comfortable with milling.

---

We don't have live tooling. It was done on the mill because plunging the very small amounts that the tool would handle would have taken too long.

 

Thad

[Thad]

Goldorak,

 

I don't follow you on the nipple being too small. Are there size limitations to face grooving?

 

Keep in mind, I'm not a lathe guy.

 

Thad

[TMozzone]

Thad,

Look at the Manchester Line of face grooving/treepan tools.

[Thad]

Will do. Thanks T!

 

Thad

[Colin Gilchrist]

+1 for Manchester

[Chris Rizzo]

we've been blowing up the manchester support blades and clamps in 4140. well actually bending them up. works ok in aluminum, thats it. even bent them in plastic, getting the chips all wrapped up. the system is just too flimsy. moved up to mitsubishi, and its a fair amount better. sandvik takes the prize though.

[Redfire427]

Your best way to cut that area is with a face grooving tool and use a zig-zag cutting motion. With a face grooving tool, your initial position for plunging is critical and you must have the proper holder for the specific job so that the clearances are correct. The problem is chip control is terrible and coolant access is poor. If you use a zig-zag motion, you completely eliminate all these issues. I do parts much like the image you have provided frequently. Iscar and Sandvik make some very nice face grooving tools.

[Barry]

I do a part very similar to this also. I use a face groove tool and my pocket is 1.65 deep and my small diameter is 1.27 my large is 2" I agree with the above post and you can clear the stock out in depth cuts.

[Redfire427]

In my post above, I am not suggesting using a grooving cycle with depth cuts. What I program is a roughing toolpath with zig-zag cuts. Although using depth cuts on a grooving cycle will work, it brings its own difficulties as well as increased cycle times due to retracts and clearances. If you have not tried my method before, give it a try. I think you will be very pleased with how well it performs.

[Jeremy Grigsby]

What about a forward facing boring bar with a 35 degree insert? Kennametal makes one thats .75 diameter i believe. I use a 1 inch bar to rough out stuff i normally would have to use a face grooving tool for. I don't get the chatter and the long wide chips wrapping around the tool. The tool im refering to stick straight out from the end of the bar minus a 5 deg clearance angle. I have a left and a right and can rough from one side with one and then the opposite side of the groove with the other. I use lathe rough, and select facing as the direction.

Usually I draw in a 45 degree line on the non cutting side of the profile. You will have to make a custom tool profile because mastercam doesnt have any of these tools in its kennametal library.

PS- I'm not at work so i can't pull up this file. I'm just going by the shape, I dont know if the size of the tool I mentioned will fit

[Andy]

Jeremy, That boring bar is a BHP-EC-600, Kennametal. It is 5/8 dia. and uses a 35 degree insert. I have used it many times. Might work good on this job for boring out the bigger ID and leaving a 45 deg. taper on the plug and then using a second boring bar to turn the OD of the plug in the center.

 

Depending on the depth of the groove one might have to use T1 then T2 then T1 again and T2 again.

 

In lathe rough you can change the angle you rough turn taper type toolpath. In this case a rough bore angle or rough face angle. You have to play with the settings until you get the path you want.