advice for o-ring grooves in stainless

[Sbarner]

We cut alot of o-ring grooves here, and I'm just curious what everyone's method is for cutting these, specifically in stainless. The groove I'm cutting is a -134, so we're talking about a .118 wide groove by .077 deep (or so). I have the heebie jeebies of plunging a 3/32" endmill into stainless. I've done it, but even at 1 IPM, the cutter is usually shot by the end of the groove. I was thinking of doing a contour ramp with a .025 ramp depth. I'd love to hear anyone's advice. This would be on a Haas VMC with Mastercam X5.

[K2csq7]

A while back I had some 5/16 deep custom oring grooves in Nitronic (worst material ever). The dovetail tool (custom) could only get in and out of the groove at 1 place (an entry location I ramped out to .471 dia.). (the grooves (2 per part) went around a large part and if you laid the path flat it was something like 150" long. What I ended up doing was 3.0 IPM 1800RPM with a 5/16" Primary Cutter Supermill (tried like 6 others nothing came close). Stepped it down with two equal steps then took a finish pass for the last .02 or .03. Then came the dovetail tool 1 pass through the middle, then stepped it over to each side for roughing, then just comped it in to get the final width. Oh yeah, 32 finish on the bottom and 63 on the sides +/-.002 on the width and the depth.

 

Good luck I hope I never have to do that again!!!!

[MBlair]

Contour ramp is the way to go.

[BissTool]

Contour ramp is the way to go.

 

 

Ditto.

[gcode]

I draw a C/L the break a 1 to 1.5" segemnt.

then I extended the main portion 1/2 the tool diamamter +.05"

I use a contour ramp on the short section to zigzag back and forth to the bottom of the slot.

then I a new operation, I china the main C/L and use a regular contour with appropriate depht cuts to rough out the main portion of the slot

 

Keith.. those O-ring groove sound exactly like the o-ring groove I was doing in 304 SS weldments.

over 800" of them per weldment, some of them with Ø1.5" dia 14" gage length toolholders .. a real PIA

[Goldorak]

Nitronic (worst material ever).

 

 

 

no , nitronic cuts like butter.....compare to stellite, A-286 and Hastelloy C276

 

we cut that stuff everyday here

 

for grooving ss304 grooves, i use a small ramp ans A LOT of coolant, you got to avoid plunging of cut with a too slow feedrate, the material will burnish and after this , it will be nearly impossible to cut

[Sbarner]

Thanks for all the advice. I think I'm going to ramp it.

[Elmer Fudd]

Drill a entry hole with a carbide drill then do a contour ramp to clean up the drill point. for the groove do a peelmill toolpath.

[Guest]

I NEVER bother with entry holes any longer. Waste of machine time from my experience

[Jayson Kramer]

I to go with ramp with a finish path at the bottom. I am intrigued by gcode;s way but I try to never if not needed to draw extra geo and most defiantly try not to draw my paths

[Sbarner]

I NEVER bother with entry holes any longer. Waste of machine time from my experience

 

Are you talking about a toolpath similar to this, or all toolpaths in general? Usually I drill an entry hole in stainless or mild steel for my entry moves in a 2D contour toolpath. I found that I have to plunge the tool at like 1 or 2 IPM to not bust it (even a 1/2" endmill). So, for me, it's just as easy to setup a drill and make a start hole. In pocketing, I use the entry motion. I tried the start hole toolpath, but that was a complete waste of time, IMHO. Creating new machine groups and making like 4 start holes for one toolpath was a joke.

[K2csq7]

I think he is talking about drilling the entry hole. Extra tool, extra offsets, more toolchanges....= more chances for mistakes & lost time & $$$. Gcode uses a line to ramp back and forth to get the tool to depth, I ramped a circle, Jay Kramer ramps the entire path...to each his own. It really depends on the individual application.

 

it's just as easy to setup a drill and make a start hole

 

If it's high qty. you will loose time + you still need to deal with the drill point at the bottom 1 way or another...

[Sbarner]

I wasn't clear in my post. I was wondering if he shunned the start hole for a toolpath like this, or for all toolpaths in general.

 

I have no doubt that you'd lose money. I'm just wondering how one balances drilling the start hole versus having to plunge the cutter at 1 IPM so that you can make it last for more than 5 parts. In other words, what technique works best for getting an endmill into mild steel or stainless using a 2D toolpath. If I want to contour around a part to cut it out, I don't want to plunge the cutter in that slow. There is no entry motion dialog for 2D contour. I'd use ramp to cut it out, but when using ramp, the tool doesn't retract for chip clearance AND you can't use tabs. So what does one do in a situation like this?

[K2csq7]

I ramp circles almost exclusively for things like this, an extra toolpath, but if you play with the linking params & lead in / out on both ops you can get the tool to ramp the circle for entry, then just start the contouring path right from the bottom of the hole you just ramped. I agree with you that plunging straight down into solid stock is not the best entry motion for tool life. You have to have the right size cutter for the entry hole you want to put in, here is the formula I use to figure cutter size vs. hole size when using inserted cutters.

 

Minimum Hole Dia.:

(Tool Dia. x 2) - (1.5 x Insert Dia.) <<<<<<Insert dia. = width of insert

 

 

Maximum Hole Dia.:*

Tool Dia. x 2

 

* Not recommended. At this diameter, the center tip is at its maximum. It is suggested that you stay slightly under this number.

 

For a centercutting end mill I always get great results using: Tool Dia X 1.5 = perfect hole size

 

 

 

 

 

[ktd]

Purchase a cheap boring head and use a face grooving tool and do it all in 1 shot.