Secondary Air Drill

[Toaster]

Yeah, I had a thought about that. I figure once I nail down this code I can just change the logic to look at tools 31-41 or whatever range I want. That would be pretty easy to implement. Although most of the jobs I run are just one drill bit at a time, I rarely change drill bits mid job.

I'm starting to realize that Vectric not outputting a real drilling toolpath is making this difficult... See this thread:

http://forum.vectric.com/viewtopic.php? ... 14&p=21174

As I see it right now I could:

-Use this hacky IF statement situation I have now. It's workable, but it makes really ugly GCode.
-Just make two post processors, one for drilling and one for cutting (but that's no fun is it!)
-Get Centroid's software to consider certain tools "drills" and fire relays for me like the ShopBot software does

The last solution is the most elegant as you can run a combo spindle/drill job in one file. It's also one that will play nice with Vectric's faux "drilling" toolpaths.

[Gary Campbell]

You need to scour the manual, or programming to see if there is a way to toggle an output based on motion or speed for a monitored axis (Z). Or take the simple way and turn the drill on before the drilling cycle, and turn it off when done.

[Toaster]

I've scoured and I can't find anything that sits and waits for a certain axis position to do something.. The closest I've found is M100/M101. They wait for an input or output to be triggered. As far as I can tell that M command can't be used for monitoring an axis.

I know I could turn the drill on and just leave it on, but when I'm doing stuff like this it would use so much air:

https://photos.app.goo.gl/vcRVqsLcT54pruzQ7

[Toaster]

Ok, I finally solved this in a practical way.

With the help of Gary, I realized that it was best to treat the air drill and the spindle as two separate tools. Essentially think of them as selectable tools in an ATC machine. The easy part is measuring the tool height, the harder part was solving the XY offset between the air drill and the spindle.

Here's how I solved it: First I measure the tool height for the spindle (T1) then for the air drill with the drill down (T2). Then I measure the distance in XY that the air drill is behind center point of the spindle. I save those air drill offset files in Centroid as #150 and #151.

I modified the post processor I use for my CAM software to run a G52 offset when I'm using Tool 2 (the air drill). That G52 offset references #150 for X and #152 for Y. If I'm using tool 1, G52s are cleared.

The last part was dealing with the two relays that operate the air drill, one drops the drill down, one spins it. At each tool change I have the Z go to the top (machine 0). When Tool 2 is called, the drill drops down. My cam software has a setting for "plunge height" At that height, if it's on Tool 2 (the drill) it'll fire the second drill relay and drill the hole. It'll dwell at the bottom of the hole and pull out. The spin relay kicks off, the drill rapids over to the next hole and at the plunge height it kicks on again and drills that hole.

If I switch back to T1 the drill retracts. Here it is on a bench test:

First here's how I zero my drill and spindle: https://photos.app.goo.gl/aQ1ghaduDrFaeDY47 Remember each tool is loose and chucked up into the spindle and drill at each job, so I need to re-measure each time I do that.

Next, here's a test drilling/cutting job where both tools are in play: https://photos.app.goo.gl/zrP8Af9DSUefRhMA9

Now that I have this out of the way I'm really close to putting this control in my machine!

[Gary Campbell]

Congrats Eric... Looks like you are ready to "Ditch the Twitch" (the movement to replace the twitchy unreliable ShopBot controller)

#ditchthetwitch

[Toaster]

Well, there's one thing more I need to get solved... squaring. I'm tempted to build my own script to do it.. But from what I hear that's coming in a update very soon?

[muibubbles]

This is interesting as I have an air drill that came with my table but never used it. I took it off for the ease of the retro fit.

If I understand correctly, you doing all the drilling operations first then all the cutting operations second correct?
What is the benefit of the air drill vs using the end mill to make the holes? Accuracy? Cost from consumables wear?

[Toaster]

A bit of an update: I simplified the code even further for this. Post processors are now all stock Centroid. The only thing I modified was the M6 tool change script. It's really simple, if tool 2 is called (the drill) it drops and spins the drill. It also applies a G52 offset. It uses a stored tool heigh measurement that I take with my touch off plate. Dead simple. It's about 5 lines of code to do this.

With this setup I can call the drill anytime in a file, one single file too, I don't need to save out two different toolpaths. I can use any CAM software that has a Centroid post.

Personally I like the drill a lot. I know that an ATC tool is better, but for the price I paid for this drill it's more than paid for itself.

For me in particular I like to drill a fair bit of undersized and oversized holes. Because it's got a regular Jacobs chuck I can put any bit in there that I want. Also, I cut with a lot of down spiral and compression bits and you don't want to drill holes with those (you'll get fires).

[mattm]

This is all very insightful - I'm just about to start working out how to setup a drill block with 8 or so actuators (using Oak and PLCADD1616). I also use Vectric amongst others and it seems really good that you managed to use the stock post processor.