Peck drilling and spindles?

[johnm]

Folks -

We are expecting delivery of our 'bot on 11/4 - YIPEEEEEEEEEEEEE!!!!!!!!!!!

Okay, breathe..... A question that popped into my head - I understand that straight plunges with a spindle are a no-no.... So, if that's the case, how the heck to you peck drill for shelf holes and the like with a spindle? Wouldn't a brad point bit cut well enough to reduce any end loads? I sure as hell don't want to damage the $$$$$pindle! Any takers??

John Moorhead

[benchmark]

Hi John,

You will not be disappointed, the increase in your production Is like another employee except it doesn't come in late or go home early and need holidays.
Peck drilling will depend on your tool-path software I use Artcam which has a peck drilling strategy as most do.

What I find really good for cabinet shelf holes is the drill press tool in the Shopbot software, it has a peck drill and a pocket function.

I have had problems on coated boards with Brad point cutters which has a spur, they seem to cut the face veneer into a washer shaped disc which spins with the cutter till it burns and then disintegrates

[benchmark]

Hi John,

You will not be disappointed....peck drilling will depend on your tool-path software I use Artcam which has a peck drilling strategy as most do.

What I find really good for cabinet shelf holes is the Drill Press tool in the Shopbot software, it has a peck drill and a pocket function.....you will not need to draw vector first just tap in a few details....give it a try.

I have had problems on coated boards with Brad point cutters which has a spur, they seem to cut the face veneer into a washer shaped disc which spins with the cutter till it burns and then disintegrates.


Paul

[richards]

John,
Here's how I modify the code. Sample 1 is straight code from PartWizard. Sample 2 is the same code, modified to peck drill.

SAMPLE 1
' Drill without pecking
J3,1.00,1.00,0.25
M3,1.00,1.00,-0.50
J3,6.00,1.00,0.25
M3,6.00,1.00,-0.50

[cip]

John
Correct me if I'm wrong but I think your original question was what about the bearing issue and a spindle. The answer is a second z head like the drill head that ShopBot sells. It is made for drilling and nothing else. The drill head takes most of the plunge load away fron the spindle.

[gerald_d]

"Peck drilling", as I understand it, is used to clear chips out of deep holes. Surely shelf holes are not that deep? Or, is there something more to be understood by peck drilling? (I don't see that peck drilling reduces a spindle bearing loads unless the cutter would have been very clogged in a deep hole).

[richards]

PDS Colombo has a 'cutter entry angle' chart that can be seen at http://www.pdscolombo.com/cutting_entry.htm. It shows that at 90-degrees, the z-axis feed speed should only be 10% of the xy-axes feed speed. It also shows that at a ramp angle of 20-degrees or less, the z-axis feed speed can equal the xy-axes feed speeds.

In practical terms, I usually set my z-axis feed speed to 0.25 - 0.5 ips when plunging and 6-ips when ramping. I use a peck drilling cycle when drilling with a cutter larger than 5mm or deeper than 0.4 inches. Whenever possible I cut a circular pocket instead of plunge drilling. That requires slow z-axis feed rates to get a round hole (0.25-ips in many cases). There's nothing scientific about my method. It was arrived at by trial and error, listening to the cutter and feeling the temperature of the saw dust. If the saw dust is too warm, I peck drill. If the cutter noise seemed to be too high, I slow down the feed speed.

Peck drilling is much slower than plunge drilling, even with my routine where I jog the z-asis to clear the chips and then jog back down to a point just slightly above the uncut material.

[gerald_d]

From a bearing point of view, it is better to load/unload the bearing once as opposed to a couple of times - unless the multiple loadings are a lot smaller than the single one (which apparently is not the case)

[richards]

Gerald,
You've got me thinking that it might be time to add a second z-axis for drilling.

[mikejohn]

Gerald, I thought the problem was the load over time with a continuing z movement might have the load increasing, whereas pecking had a light load.
However, you know how knowledgeable I am on engineering.

for years I thought torque was what Australians did when speaking!
.............Mike

[gerald_d]

Mike_R, I am not saying that you must not drill with a spindle. I am simply questioning the concept of peck drilling and how it is supposed to save bearing life.

Mike_J, whether pecking a hole or drilling it one-shot, the total energy (or work) required is the same. (Except for blocked flutes in deep holes).

Some cutters are especially designed for end-drilling, while others will refuse to drill at all - I cannot understand Colombo's blanket rule of thumb to have vertical plunge speed at only 10% of horizontal move speed. That is a very conservative approach.

Our default cutting tools today (>90% of our purchases) are 2-fluted solid carbide "slot-drills (http://www.google.com/search?sourceid=navclient&ie=UTF-8&rls=GGLD%2CGGLD:2005-07%2CGGLD:en&q=slot%2Bdrill)" because of their low cost and reasonable cutting performance (Plus the locals are geared up for resharpening them economically). They plunge very easily and we will probably plunge at 50% of move speed when they are used in the spindle. We will keep an eye on bearing life and may change the bearing configuration if thrust loads are a problem for our spindle - Fimec has a couple of bearing options available. (This also illustrates the danger of extrapolating Colombo specs to all spindles - they are not all the same).

[mikejohn]

Gerald
I have just 'Googled' slot drills, and come up with something described in parenthesis as an end mill. Look here, great discounts (http://www.lawson-his.co.uk/scripts/products.php?cat=Carbide%20Slot%20Drill)!
Some appear tapered though. Can you cut material, say, 30mm thick with these?
What materials are you cutting with these?
.............Mike

[gerald_d]

I am not familiar with tapered slot drills - maybe an illusion in the pics that you are seeing?

Our 10mm slot drills have a 22mm long/deep cutting edge. We typically do 30mm in 3 passes, but 30mm is rare for us. Mostly cutting MDF and ply.

Slot drills are primarily used by the metalworking industry to cut things like keyway slots in steel shafts. They are only available in up-spiral and obviously don't leave a top quality top edge in wood.

[mikejohn]

Can you get different sizes for different collets?
1/4" or 8mm?
Are you buying them locally?
..............Mike

[gerald_d]

We buy them locally, but I believe this (http://www.yg1.co.kr/main2-english/object/object-1.htm) is the source company in our case. The style is very common to many manufacturers.

Many sizes available:
from 1 to 10 mm in 0.5 increments
from 10 to 20 mm in 1 mm increments
etc.
Also some inch sizes.

I will be surprised if nobody stocks them in your town - these cutters are extremely common for metalworkers. (Though the name "slot-drill" might not work in your part of the world).

[evan]

It's my understanding that Peck Drilling is, as Gerald says, to clear chips there by reducing heat and prolonging the life of the bit. I can't see any reason not to plunge a spindle or a router as long as the bit is designed to plunge and isn't greater than .375". If larger than that I Pocket the hole.
Some times if it'll save a bit change I'll even pocket a .375" hole.
If you're cutting a profile of a square to a depth of 1.5" and you ramp into the cut, more than likely you make the cut in multiple passes and each step will be a plunge after the initial ramp. Or are you guys ramping down for each step of the cut?

Evan

[richards]

I ramp on all passes.

[wemme]

I Never Relised Drilling multiple hole was bad for the spindle. I thought the brearings would have been designed to handle the up/down forces. I Havn't needed to do this yet but is good to know.

[Norm (Unregistered Guest)]

So a spindle would not be a good for plunge roughing either?

[richards]

Taking the time to add a software ramp for each piece in your part file is a trivial matter. The advantages inherent in using a spindle compared to using a router far outweigh the disadvantages. The procedure that I normally use in PartWizard is to set the starting point for each piece to a point where there is a straight-line portion long enough for a ramp and then add the ramp manually when I combine the various SBP files into a master SBP file.

I understand that the higher priced versions of tool pathing software can add ramping automatically.

[earld]

Better late than never:
Peck drilling in the metal machining world is used to break the chips that would otherwise become long stings of razor sharp snakes that destroy people and machines.
The two types of peck drilling I've seen in CNC routines both are chip breakers. One type will make a cut to a preset depth then reverse feed .005" then resume to the preset depth. Because of the spiral on the drill/cutter the chips will be cleared from the hole. In cutting cast iron or other materials that can be gummy, the other peck drill routine will drill a preset depth and jog from the hole to clear the chips and then resume the feed to the drilling depth previously established by the preset depth, until the hole reaches design depth.
In the wood world, if you are using a spiral up cutter and the chips (sawdust) is/.are coming out of the hole without loading the cutter then there is no problem.
Straight flute cutters need to have a peck clearing routine.
Don't know where the concern for plunging is coming from, probably an urban legend. Spindles are built with high quality thrust bearings that should take thrust loads much better than the side loading from the normal cutting and shaping operations. If not, then someone is selling a poor quality spindle.

[richards]

Duane,
PDS Colombo has a differing opinion about thrust loads and the bearings used in their spindles:

"Electric Spindles designed for routing applications are equipped with bearings capable of enduring high radial loads (side cutting). When entering the work piece with these spindles it is important to keep the axial loads low in order to prolong bearing life.

When programming your work-piece, entry angles should be kept from 0º - 20º off the table. This will keep axial loading low and allow feed rates at 100%.

When the work piece design requires a steep entry angle, the feed rate should be reduced according to the chart. This will minimize axial force on the bearings." (www.pdscolombo.com/cutting_entry.htm (http://www.pdscolombo.com/cutting_entry.htm))