bell-mouthed holes

[snowshovelbmx]

I am drilling some 1 1/16" holes through some material at work with a spade drill and am having trouble holding even the .01" tolerance. The holes are about 1.08 on the near side and then 1.065 on the far side. Obvioulsly the drill is walking into the hole before finding center any ides on how to stop this?
The material is just normal cast steel not sure of a grade. The drill is an 1 1/16" allied spade drill with a TiALN coated HSS insert, I am running the drill at 180 SFM (680 rpm) and 10 IPM (about 0.015"/rev) 4 of the holes are 1.25 deep and the other is 4 inches deep all thru holes. The machine is a DHM 680 horizontal machining center with a cat 50 taper spindle, so plenty rigged enough. Anything else? Any ideas?
thanks,
chris

[g-codeguy]

Have you tried a much slower feedrate to get the hole started, and then kicking the feedrate up?

[TOTALLYRC]

Originally Posted by snowshovelbmx I am drilling some 1 1/16" holes through some material at work with a spade drill and am having trouble holding even the .01" tolerance. The holes are about 1.08 on the near side and then 1.065 on the far side. Obvioulsly the drill is walking into the hole before finding center any ides on how to stop this? The material is just normal cast steel not sure of a grade. The drill is an 1 1/16" allied spade drill with a TiALN coated HSS insert, I am running the drill at 180 SFM (680 rpm) and 10 IPM (about 0.015"/rev) 4 of the holes are 1.25 deep and the other is 4 inches deep all thru holes. The machine is a DHM 680 horizontal machining center with a cat 50 taper spindle, so plenty rigged enough. Anything else? Any ideas? thanks, chris

I am sure that I am missing something something, but are you spot/center dirlling first?
Mike

[snowshovelbmx]

i am going to play around with it today. I will try a slower feed to start but it is going to be a production part so I would rather not do that in the end. As for spot drilling I had one in there at first but spade drills really are not supposed to run with a spot drill and it seems to not help so that is gone now. Thanks for the replies.

[LeeWay]

If it has to be that precise, can't you use a smaller drill to start with? Say a 1". Then you could use a boring bar to finish it up to get it just right. I know that is two steps, but if you want precise holes, this is the most repeatably accurate way I know to do it.

[fuzzyracing1967]

Have you checked to see that the drill runs true? If the drill runs out just .005 it will cut big untill it gets into a full cut.
The other thing that comes to mind would be if the part was held tight? You say the machine is rigid but how about the work holding,some times it's the little things.

[Delw]

Alot of it may have to d with a chipped or even point on your drill, the other thing That I have had problems in the past with is the face of the part is un even. this will cause a 3" dia bit to walk off a tad and cut funny.

Check to make sure you face of the part is flat/squared with the spindle, if its not there is your problem.

[snowshovelbmx]

thanks for the replies, as for boring the hole that wont do, these are production parts and the one hole is 4 inches deep. I should be able to hold the tolerance with a drill. The runout on the drill right at the insert is only .002" and it is a band new insert. The face of the part is milled right before drilling the holes, in the same set-up so it is square/true. As for the setup being rigid the facemilling that I just mentioned is being done with a 3" facemill full width and .200" depth of cut so it is plently rigid. All that I can think of is that the drill, being a standard length, is just too long for it to start correctly..for now we are using a 3/4" endmill to helix bore the hole .625 deep and then drilling. I would not like to do this for prodution though....for the sample part it is fine. Allied recomendes spoting the hole with a spot drill of equal or greater included angle than the drill? anyone ever done this?

[ALLtra Mach]

Yes, you can spot drill for spade drills, as long as equal or greater angle.
Also, Allied recommends speeds up to 470 SFM for that drill. The speed your running is for a hard material. I would try more Speed first.
Your big to small hole is definitely from walking.
And yes, with that drill you should easilyu hold the tolerance. Getting ahold of Allied was the best thing you can do. Which is something I see alot of on here, your first step when having problems with a tool is contact the company rep. Nobody should know those tools better than them.

[snowshovelbmx]

Ok thanks a lot! I will try that soon. whenever we run the next set of castings...as for the speed on that are you sure of the 470 sfm? I am using a coated HSS insert not a carbide one. Thanks.

chris.

[ALLtra Mach]

Ummmm....Ooooops.....wrong chart LOL
http://www.alliedmachine.com/Technical/TAInchSFHSS.cfm

Yeah maybe around 250sfm would work better.
Sorry!

[snowshovelbmx]

yeah thats what I was thinking, thanks. I will let you know how it works when I run them. We might just be getting a u-drill which would solve the problem...faster too!