I use the circle function to drill .030" holes in the PCBs that I produce with CC. I set the radius of a circle to .001". The barely perceivable oscillation doesn’t break my very delicate .030" bits so I don’t think it will bother anything else. I broke several bits drilling by hand but haven’t broken 1 doing it this way. The only draw back is that I can’t see the “circles” I’m making because they are so small. I solve this problem by first locating the holes with larger circles that I can see. I then create a circle with a .001" radius and locate it at the center of a large circle, then using the “rubber band box” I select and copy (command/C) the little circle (visible as a node) and move the copy to the next large circle center. Repeat this copying process until all holes are positioned. Now delete the large circles using the rubber band box to select as many large circles as possible touching only the very edge of the circles. I have a Mac so I use the “delete” button located with the “home”, “end”, “page up”, “page down” key pad. Go to “tool path” and select all locations with the rubber band box and set the parameters of the tool path to your requirements (speed, plungerate,etc) but be sure to select “NO OFFSET”. Then click OK. Check tool path by hovering over the tool path with curser.
This probably sounds like a long way to go but, believe me, compared to hand drilling 100 holes or more every time I make a new board, this is a piece of cake.
I make this tool path a separate file so that after I complete the PCB, I can change the tool to a drill bit and re zero my controller and select this file to drill the holes.
(Can CC be modified to use a “circle” with a 0.0 radius and indicate it with a cross hair or x?)
NOTE: I have an off line controller so I don’t use Carbide Motion. All I need are the G-code files to plug into the controller. I don’t know how computer software output might differ.
How does that work? Do I draw up what I need then upload it to the web page? All I need are G-code files. With CarbideCreate I do everything on the same software. I don’t have to import anything or manipulate anything to get it to work. Besides, I do a lot of other work on my router, not just PCBs. I was really only replying to several other comments I’ve read about drilling holes with CarbideCreate. I’ve been able to get it to work and thought someone else may be interested. If I can get it to work, anyone can. I’m a machinist, not a computer wiz.
Carbide copper is useful if you design your PCBs in different software. Sounds like you’re drawing them by “hand” in Create?
How do you generate toolpaths for a .030" bit in a .001" hole?
Instead of making small circles in larger ones, you could just tell CC that you’re using a larger endmill. Make the hole slightly larger than the mill and it will bore a hole. You’ll get the same motions with a smaller tool loaded(smaller holes).
If you’re designing PCB’s entirely by hand in CC, it’s “the hard way” - that’s more easily done with something like Eagle (that already has all the parts and pads in it’s library, and can often autoroute for you), then you can import the gerber files that Eagle generates into copper and it’ll take care of the hard work around setting up both the etch and the holes. Copper then outputs the g-code files for the machine for the various tools. Copper can be used to either process gerber files from something like eagle, or you could design the whole board there. Whatever works for you.
You created a new thread, so I assumed you were looking for a different way.
NO. I was just illustrating what one can do with CC if one wants to. After many weeks of trying to get other software to work at all, I was so impressed with CC and its simplicity to learn and use I just wanted to tell other users about it. One of the topics that has come up in the past (many times) was the lack of a drill function. Since I have been hand drilling my prototype PCBs for decades (and breaking lots of bits), I thought this was a feature I would like. I tried tricking the circle function into thinking it was making a very tiny circle, and it worked. Now, in the time it would take to hand drill one board, I can make a G-code file to do it automatically for as many boards as I need.
If you have a system that works for you, that’s great. I’m not trying to convert anyone.
Now, I have a question. While working on the web page, would I be streaming data? I’m not a computer geek and don’t understand much of what I know about online operation. What I do know, is that I don’t need a web connection to use CC.
As for the drill size, that is the size hole I need and no bit that size or smaller could withstand the side load of milling a circle. The bit must travel straight down with as little side load as possible. A .030" bit is very tiny and brittle. I haven’t broken a bit yet
I think I get what you did. You had the drill cut a profile around a very small circle. Interesting solution. When you referred to the “holes”, it makes it sound like your creating a small pocket (boring).
That’s exactly what it does. Because my holes have to be so small, the bit has to go down as straight as possible. when working, it looks like an automated drill press (much like your video). I too feared that the circular oscillation would snap the .030 bit I needed to use, but it didn’t. If I were making larger holes I could use an end mill and simply mill the holes to size. I figured the tiny holes would be the worst case scenereo due to the fragility of the bits.
P.S.: In reference to the larger circles. When you try to apply a circle with a radius of .001", it is not visible on the grid. I use the larger circles for layout purposes only. They give me a visible target to locate the “invisible” holes. That’s why they are deleted from the tool path.
Can’t you just draw 0.031" pockets and do a pocketing operation? Then you could most likely see what you’re drawing and the 0.031" versus your 0.030 tool would cut essentially the same way as with the 0.001" holes with a profile cut. Maybe I’m missing something?
Makes sense when you’re doing a tiny profile. Most people use the solution of boring a hole as a tiny pocket, just larger than the bit. As @DanoInTx said, the end result in machine movement is exactly the same. My reference to using larger circles was to solve the problem of not seeing the tiny .03" circles. Use .100" circles, but use a .099" end mill. The machine doesn’t need to know that you chucked a .030" drill bit…the result will be the same.
I tried that and it does work better. I was manipulating the function and never considered faking the tool. It never occurred to me that I could create a totally bogus tool (a non-standard size). Doing it this way eliminates the slight wobble and, of course, I can see the objects on the grid while laying them out.
This is why I started this thread in the first place. I wanted to see more discussion of CarbideCreate and the possibilities if thinking outside the box. Look, we’re talking about two ways of doing something with CC that I was told you can’t do. And yours is better than mine. That’s great!