Sorry in advance for this pretty dumb question, but I’m gonna ask it. So I’ve got a program on my 770M I’ll run to drill a bunch of different diameter holes in a plate. I’ve only got three TTS Jacobs chucks on hand, and so I’ll need to change out the twist drill several times for the same Tool # Jacobs chuck during the program. In each case, I’ll likely end up with a different Tool Length in Offsets for that same “Tool #1” chuck for each different drill that I’ll put in the chuck. My dumb question is this: is there a safe way to ‘intervene’ during the program running, to pause and input a new/different Tool Length in ‘Offsets’ for that same chuck, and then re-start the program and have it drill the next, different hole with the correct Tool Length in ‘Offsets’? I don’t know how to do that in PathPilot…I hope my question is clear, I don’t feel like I’ve expressed it real well, but hopefully you guys know what I’m asking here. Thanks–Charley in Colorado
me again–poking around a bit on the web, I find several sorts of answers to what I’m asking;
–use drill collars and simply make it such that there’s only one Offset value in the program for that chuck/Tool#, and each different drill is set with a collar to produce the same Offset…
–use ER collets to hold the drills, and just have a different Tool # and Offset for each of them; I sort of like that; I’ve never taken advantage of the ‘diameter range’ of ER collets, but I know you can do that all right; so, that would work…(if I’ve got enough of the right ER collets/TTS holders on hand!)
–post-out separate programs for each drill size–yuck, that sounds like a pain to me…
–I didn’t (so far) see a straight-up answer to my question though, i.e., how to ‘pause the cycle’ and input a new/different Offset value for the next drill in the chuck…maybe that’s just not something PP allows you to do? Thanks again —Charley
Charley, pathpilot locks down the interface such that can’t edit the tool table while running a program. Something you have already figured out. There might be some wizbangary you can do with gcode but you would need to know the lengths ahead of time. The way I would approach this is to call out each different drill size as a different tool number and then just end the program when it asks for the next tool. Then you can use the same holder but have an easy place to find where you left off to start the program in the middle. Here is a video we put together on starting in the middle of your program
Fwiw. I favor ER collet for holding drill bits. That’s an option if you have enough extra holders.
Dave, thanks for your feedback on this and the video link, too, I’ll sure check that out. Yes, I guess I can see where the PP folks are coming from on that, could well result in sort of a “crash generator” to have that flexibility, eh…! I just figured, with all the jillions of switches and knobs that populate PP, this would surely be in there somehow or other. At any rate, I’ll go the ER collet/separate Tools route, and call it good. Thx—
don’t use the same tool number for all the drills. The machine doesn’t care if you actually take a toolholder out or not. At the tool change just change bits. You can then even have different tool lengths. just bottom the drill bit out so you get a somewhat repeatable length
Thanks, Jon, I see what you’re saying there, too. In some of these drills in my setup, they may be gripping on the flutes instead of the shank, if I bottomed them out in the chuck like you describe…not sure in a case or two. But it makes sense if it works out in that regard, I can see. I think I’ll try to go the route of using ER collets to hold the drills that exceed my three Jacobs guys I’ve got, that also makes good sense. Like I noted above, I’ve never to date used my ER collets with anything other than ‘spec diameter’ tools (e.g. an 1/8" shank in an 1/8" collet, etc.), but I do know they’re designed to accommodate a pretty wide range. And maybe even a better way to hold a twist drill anyhow, which I’d not ever considered. --Charley
—this plate’s got a LOT more different holes in it than I’m used to dealing with, resulting in these tool-holding issues I’d never really come across until now! –
Even the cheap sets of collets on Amazon are likely to have better run out than a decent drill chuck. I only use a drill chuck for the occasional odd size drill. If it’s a size I run regular it’s in a collet chuck
Got it, thanks. I’m not using my ER collets/holders as much and as well as I ought to be, I’m now seeing. I just hadn’t really ever gotten the message that ER collets hold twist drills better (lower runout; grip them well) than drill chucks, until now. Onward!
–a quick related question; does using ER collets well away from their ‘nominal’ size (e.g. 1/8", 1/4", etc.) wear them out or otherwise mess them up, more quickly than if you only use them at their nominal size? I see on a nice chart I found, that ER collets consecutively ‘fill in’ the range’ of diameters completely, but, say I wanted to hold a 0.1562 drill in a 1/8" ER collet, does that more quickly wear out or bother that collet? It’s just at the edge of the 1/8 ER diameter range, but, it is in the range…? Just wondering. –
Unless your drills are Imperial sizes (1/16 , 1/8, 1/4, etc) it is better to use metric ER collets since a set of metric collets covers ALL intermediate sizes. As Jon mentioned, even cheap metric ER collets from Amazon are apt to be more accurate than your Jacobs chucks. You may want to purchase two or three sets of collets since you may need the same size collet for several different drill sizes. Standard quality ER collets are cheap!
It is not a good idea to cram a 0.1562 drill into a 1/8-inch collet. Get a 4mm one!
if you want to keep freedom units. they make 5/32 collets. Tormach has them in the store or they will come in the el-cheapo sets (I’m 99% they are just the metric set with imperial approximations laser engraved)
Thx, got it. Ie, just because it’s “in the range” of the smaller collet, doesn’t mean it’s a good idea…makes sense. I’m actually sort of surprised you can “go larger” in an ER collet (“going smaller, I can see that easily enough) but I guess you can spring them open a bit and squeeze a larger dia shank in them eh.
I have to ask what is the spead In hole sizes. The time it would take change things out could be equally uses to simplr mill borethe holes, dependingnon depth. For me, i made a bunch of TTS tool hold blanks. I have them for tap drill sizes up to 1/2-13 dedicated. Also for typical clearance hole drills. You can order blanks from Tormach but they are very easy make on a manual lathe. I also make my own ER collet tool holder but those are made on a Hardige CNC. Once I have the blank, i hold it with a small 3 jawnor maybe a v block i vertical position. Indicate the position and simply drill on that location with the desired drill for that holder. Then hold drill for a set screw. Make sure to be a few thou off center againstnthe directionnof rotation. This helps prevent loosening during operation.
Just food for thought. It works really well for me.
Do you have an electronic toolsetter? This is how I get around the problem in my shop. I highly recommend a toolsetter if you don’t have one. Extremely convenient. I have the inexpensive one from eBay and it works very well.
With the toolsetter, you would just have the postprocessor call a tool length set operation for each new tool in the setup. I use David Loomes (xoomspeeds) F360 postprocessor that has a quick check box for an optional tool length set for each new tool in the program.
Use different tool numbers for each drill. Then when running your program, PP will ask for the next tool. Put your bit in the chuck, hit cycle start, let it measure and set the new tool length automatically, and off it goes.
Thanks, no I don’t have a toolsetter, I’ve looked at them on the web but so far hadn’t thought I wanted/needed one. But I’ll look at it more closely now. –