Chain drilling - How to make Fusion drill every other hole first?

[Anonymous]

Hi!

I make jewelry rings out of slices of precious materials. I want to keep as much of the material as possible to be able to make other jewelry, so the operation I found to be quickest and most reliable is to drill a bunch of small holes using a short carbide drill in a circle with a small overlap to create a "plug" in the center of the ring, which I then can remove before cleaning up the inner surface using a large endmill.

However, I do snap quite a few drill bits and I do believe it perhaps might have something to do with unequal load on the drill bit by only having one side not engaging material. The current operation always drills the hole right next to the previous one in a circle.

My setup is a single drilling operation that I have used a folder to create a circular pattern.

What I would like to do is drill every other hole first so that the first half of the holes would be in virgin material and then followed up by drilling the next half in between those holes, which in theory would give a more even load on the drill bit? (Not sure if I'm correct in that logic).

The problem is that every I manufacture is of a different size so the number of holes drilled, and the overlap slightly varies. If it was only one size I needed to do it would be fine to do the hole positions in the sketch and then manually select the points individually in the drilling operation, but it needs to be as flexible and with the smallest chance of operator error as possible.

Any ideas?

Thanks for your time and help

(Edit: I am not an admin on this page. I'm not sure why it's showing my username as such. I've tried changing it but it doesn't seem to update?)

[Anonymous · Accepted solution]

Make 2 sets of holes that deviate in size by small value, using same size drill, first select one smaller hole and select range that omits large holes, then duplicate the operation and select holes in range that omits smaller holes.

[dylan_smith]

Hi @Anonymous,

Do you spot drill the holes? 

Going straight into the material may cause your drill to wonder of to one side which can contribute to more stress on the tool. If you spot drill the holes prior to the actual drilling operation, this may help you snap less drills. 

Thanks

[Anonymous]

Well, if your comment was inspired by the fact that I did not use spot drill, I wanna point out few things.

Poster indicated that he uses short carbide drill, given that, there are disadvantages in using spot drill.

Carbide does not flex and since he wants to save as much stock as reasonably possible, he is probably using small diameter drill.

1 - If spot drill is not perfectly centered with drill, using spot drill can pull drill off center when engaging the cut and drill will brake.

2 - If perfectly lined up with drill, spot drill would have to have equal or larger tip angle to ensure that drill engages stock with its center point or entire width of the cutting flutes.

If spot drill has smaller included angle then drill, drill will engage stock with outer edges of cutting tip, that produces chatter and vibration, vibration kills carbide.

So, best way to ensure that short carbide drill engages stock with its center point is to not use spot drill.

Use low feed rate to engage cut, making sure drill goes deep enough to form full diameter

pocket, without retracting drill, make few shallow segments while gradually increasing feed rate for each one until desired feed rate is achieved.

Depending on material, pecking can be beneficial or detrimental but if opting to peck, never retract drill fully from hole, instead retract so that tip of the drill remains below top of the hole by about same value as drill diameter.

This allows for evacuation of chips and injection of coolant while not risking chips getting in a way of drill reentering the hole and potentially causing it to break.

Pecking or not would be mostly related to how material reacts to drilling, strings of chips can plug flutes and deprive drill of proper coolant supply, pack inside flutes and cause premature damage to drill and work piece.

If using long carbide drill, spot drill would be beneficial, providing it is perfectly centered and in sink with drill.

To make sure drill engages cut with its center point, spot drill should only go so deep to create point about same diameter as width of carbide drill web thickness.

[Anonymous]

---

@Anonymous wrote:

Make 2 sets of holes that deviate in size by small value, using same size drill, first select one smaller hole and select range that omits large holes, then duplicate the operation and select holes in range that omits smaller holes.

---

Great idea @Anonymous !

The problem still left to solve is how to be able to quickly change the number of holes and have them overlap equally. I'll play around a bit to see if I can find a solution.

Thanks for the input, much appreciated.

---

@Anonymous wrote:

Use low feed rate to engage cut, making sure drill goes deep enough to form full diameter

pocket, without retracting drill, make few shallow segments while gradually increasing feed rate for each one until desired feed rate is achieved.

Depending on material, pecking can be beneficial or detrimental but if opting to peck, never retract drill fully from hole, instead retract so that tip of the drill remains below top of the hole by about same value as drill diameter.

---

 These two suggestions are fantastic! Not retracting fully and slow feed in makes total sense. I'll try that.

[engineguy]

@Anonymous 

Would seem to me that you are already close to a solution, drilling every other hole should in theory be a better way,  Carbide drills don`t like being pushed to the side, too brittle, HSS are much better in that respect, maybe this idea will work a little better for you, try doing two Drilling operations and on the first one do a Circular Pattern by selecting say the top hole on your sketch and setting the number of holes in the 360 degrees to half the amount required and that way you will drill only every other hole.

You don`t say how you hold the "plug" down, it would need to be held somehow otherwise it could easily go flying off somewhere breaking the drill in the process 😞 😞

Do the same for a second Drilling operation but this time select the next hole on your sketch and doing the same and this time it should drill the holes in between the first set.

Don`t know if that makes sense to you so here are a couple of images and the example file attached.

For different diameters/hole sizes/numbers you can either edit the original sketch or make a new one for each job which would alllow you to go back and do a job weeks/months later quickly and easily.

Hope this helps a little

Regards

Rob

[Anonymous]

I guess you'll have to do some math because I don't know what size circle you are working with, what size wholes, how many can you fit in that circle and how you make sure they overlap each other by a hair.

I was just using one way to select every other hole that happens to be in sink with options in drilling operation, the rest is up to you.

[engineguy]

@Anonymous 

Vic, I do agree with you, without an f3d file from the OP it is just "educated gueswork", we can only do what we can to point someone in a particular direction 🙂 🙂

I this instance the OP has had some alternatives to work with so as you rightly say it is now up to the OP to do the actual Math for his specific operation.

An interesting one for sure, as I have all sorts of old fashioned tooling from many years ago I would actually have tried using an old "treppaning" type tool, bit like a "fly cutter" but with a Carbide tip in a holder that can be slid along a horizontal shaft to determine the diameter required that is fastened to a vertical shaft, turn the shaft and the circle is cut 🙂

Would still need say a couple of screws to hold the piece being cut out down 🙂 🙂

Loads of ways to do the job 🙂 🙂 🙂

Regards

Rob

[Anonymous]

For all we know guy could be cutting rocks on microscopic scale, so many posters brag about their "issues", often providing no clue for someone to help them and in so many cases lock basic skills to get anything done, this is general observation and not in reference to this particular post.

It's entertaining and time filling to challenge one self with providing assistance and in many cases valid solutions that can be posted, loaded in machine and ready to produce finished component, all free of charge, although at times getting something done complete is also beneficial to advancing own skills and discovering new tricks from others involved in same tread.

In general I just want to point out that I do much more detailed and complete job for people that pay me 🙄.

[Anonymous]

This totally worked. I just had to figure out a formula for adjusting the number of holes depending on the size of the circle. I made two circle patterns with slightly different diameters on the holes. Works a treat and it's all automatic now 😄

[Stuart-H]

Taking a view from the side line 

why not just interpolate the inside dia of the ring with a small end mill using contour and a ramp feed that way you would have the left over material and the bore to size in one operation 

[Anonymous]

I would opt for drilling, small diameter drill has all its strength directed in axial cut, if end mill of same diameter is driven radially, it will not go very far.

[Anonymous]

I can report back that I'm breaking far fewer drills now, plus the automatic setup saves time and reduces the chance of human error while doing the setup.

Thanks again everyone