Page 2 of 2

Re: Interlocking parts

Posted: Mon Jul 13, 2015 12:48 pm
by Daman691003
So there's no way to get sketch up to work

Re: Interlocking parts

Posted: Mon Jul 13, 2015 12:53 pm
by Daman691003
Also won't changing bit diameter ruin rest of part.

Re: Interlocking parts

Posted: Mon Jul 13, 2015 1:48 pm
by cvoinescu
You can move things in SketchUp by precise, small amounts. You won't see the effect unless you change your settings to display enough decimals, but the change will be there in the model. Select the item(s) you need to move (e.g. the surfaces of the joint that need some clearance), move them in the direction you need, then type in the displacement you actually want, and they'll move there.

Please note that, for this to work, your machine needs to be calibrated fairly accurately: the axes need to be perpendicular to each other, the spindle needs to be accurately parallel to the Z axis, the actual measured tool diameter entered in CAD, and the runout needs to be low (or accounted for). If you want an edge milled in the X direction to mesh with one milled in the Y direction (which you'll have to do if you build a six-sided box), the X and Y steps-per-mm need to be calibrated so that the two axes travel exactly the same.

Also, you need corner relief for many CNC machined joints. (You probably know this and have already accounted for it, but I didn't see it mentioned.)

Re: Interlocking parts

Posted: Mon Jul 13, 2015 2:15 pm
by Woodworker
If you change the bit diameter it will be the same for the entire part, so it should still fit together. If you are doing engraving or clearance openings you would not notice the difference. If you are making holes for switches or such, just make those as a separate operation and don't adjust the bit diameter. I normally break the milling into operations I can do separately. That way is one of them is off, you can adjust just that operation.

Re: Interlocking parts

Posted: Mon Jul 13, 2015 4:27 pm
by TDA
DanMc wrote:Actually with CamBam I would leave the bit sizes alone, even check them with a micrometer if you have one. You can over/undersize using the roughing clearance parameter. Although better still would be to deal with that in CAD so the rest of the part is not effected.
I realize that this isn't exactly the topic of the thread. However, NEVER mic a carbide tool. Doesn't matter how careful you are or if it looks like you haven't done damage you almost certainly have. Attached is a picture of one of our 0.0280" tools that someone tried to measure with a micrometer. There was no damage visible to the naked eye. The damage done to this tool though is more than enough to effect bit life and cut quality. I apologize for the image quality as this was on one of our old tool makers scopes before we upgraded it.

Additionally, You won't get a perfect measurement anyway due to the tool runout. Basically if one of the flutes is longer than the others than that flute alone will determine the max size of the cut. So, if the tool has a flute that is 0.001" wider (from the center of the bit). It will add that much to the other side of the cut as well. Possibly not a huge issue depending on the tolerance you are trying to hold.

Just to be clear I'm not trying to beat up anyone here. I just want to make a clear point of the risks of doing this. I've seen quite a few tools die an early death from people trying to mic them.

Re: Interlocking parts

Posted: Mon Jul 13, 2015 4:59 pm
by Hans
TDA wrote:NEVER mic a carbide tool.
Thanks for weighing in, expert advice is really helpful. Do you mean to imply that it's okay to mic a steel tool? Also, can one mic a tool back at the shank where there's nothing to chip? None of us have tool scopes, so I'm looking for a better way to find offsets other than test cuts.

Re: Interlocking parts

Posted: Mon Jul 13, 2015 5:31 pm
by TDA
I don't have a lot of personal experience in HSS tooling as we only make carbide. In general HSS is much tougher than carbide although not nearly as hard (hence the much longer tool life and higher cut speeds of carbide). However, In general any sharp cutting tool is going to be damaged by taking a micrometer to it. Basically a sharp tool has as thin a leading edge as possible I can't really imagine any material holding up to it that is that thin.

You can safely measure the part of the tool after carryout (the part with no grooves cut in it). If a tool has been plunge ground past the carry out this will give you an idea of the MAX diameter of the tool. However, if the tool has a relief grind in it (a final grind on the edge of the tool from the outside) than this number will always be a bit large.

One other thing to keep in mind. Your total cut diameter is a combination of multiple factors. Tool diameter, TIR, material flex, even running a well used tool can effect the final cut diameter. Additionally, defection and out of square spindles can produce a taper. While this is not a true change in cut diameter it can also produce a similar effect depending on the code.

Unfortunately this basically means that the same tool in different machines or different materials can change your cut size. The best way to tell is to make a test cut.

Hope that helps. I'm usually hanging around so if anyone needs anything else or wants a more detailed explanation let me know.

Re: Interlocking parts

Posted: Tue Jul 14, 2015 7:20 pm
by Gadgetman!
That endmill looks as if someone's been chewing on it...

Did a bit of calculation...
0.028" = 0.71mm.

Re: Interlocking parts

Posted: Tue Jul 14, 2015 10:30 pm
by TDA
"The mic dog ate my tool!"

This particular one is on the smaller size. However, the important thing is what is done to the leading edge. The same thing will happen to a 1/2" tool (assuming that it's sharp). It will just be harder to tell... other than it's going to die quicker and most likely give you a worse cut and deflection.