Printable View
I set up models for a punch and die with 0.004" clearance. When cut out on a CNC I couldn't fit the parts together. I did the finishing light pass climb cutting. I need to do some measurements but apparently the end mills don't cut quite as big as the nominal size. Someone suggested doing a test pocket of a simple shape to check how close to size the milling will be. Can someone enlighten me on some ways to deal with this issue?
Very carefully measure your endmill and plug that value either into your CAM program or adjust your cutter comp in the CNC program. Normally endmills run a bit small, especially carbides. I use a lot of 1/4 inch solid carbide router bits for metal work, and you can count on those being between 0.246 down to 0.239. No problem, you just compensate for the size.
Good to know. I will measure those. I think some may be due to cutter deflection. My final pass I did with an 1/8" end mill. About 1" hanging out of collet (just a rough guess). I was aiming to be very conservative on feed and had coolant system running. 5000 RPM, 5 IPM, DOC 0.030. Climb milling on last pass which I just saw gives worse deflection than conventional. I left 0.020 radial stock on the previous pass but with a 0.25 cutter so there was more on some corners. From just a quick look on google it appears the deflection of the cutter is less than your numbers for variation in cutter size. I was climb milling for a better finish and (hopefully) less crud on the top edge - I need a crisp upper edge. I could have made a pass with the 1/8 cutter to leave a consistent amount and then a finishing pass to remove the last but not sure if that is needed...
The end mill is 0.123 so 0.001 undersize on the radius. On both parts that adds up to 0.002 which is half my clearance. I am guessing deflection took up the other half but haven't found any free deflection calculators to plug the numbers into. I could put the end mill farther into the collet and reduce the length to about 0.5" which will reduce whatever deflection there is significantly.
I measured the male and female across flat sections. The female is within 0.001 of desired - at least with a caliper. The male is where all the error is (I should do a more accurate measurement). I cut the male last and had reloaded the end mill but it seems strange that I got that much difference.
Just went back to double check the two CAM setups and found a difference between the male and female feed and DOC. The female is 5 IPM and 0.030 DOC. Male is 7 IPM and 0.042 DOC. Perhaps deflection is the issue. End mill is carbide.
I had some other issues with the male half (my errors in setup of some drilling operations) so perhaps I can just redo the male half. Anyone got a deflection calculator that can run the numbers to see if this is reasonable?
When using a 1/8 end mill, leaving a bit less for final cleanup might be in order. I would normally leave about 0.005 - 0.010 to minimize tool deflection. Making a second cleanup pass might help also.
I also see that there is an option in the CAM for a "spring" pass. Basically going over the same path again but just removing what was left due to cutter deflection. I looked for a deflection calculator/estimator but didn't find any free ones on line or for download. I am thinking I could also make the cuts and then measure while still located on the mill and rerun and/or adjust as needed.
That is exactly what I do on critical dimensions.Quote:
Originally Posted by Jim27
Someone ran the deflection for me and it was VERY small. But I didn't see any other explanation so I added a spring pass and reduced the tool length as much as possible (about 1/2 inch). I still got 0.006 excess material all the way around. Measured in two different places across flats. So it appears to be something in the CAM and gcode. I put in -0.006 'stock to leave' and things came out as needed. Still not sure why this was off. Looking into the CAM end of things...
There is always some deflection and spring in the machine, but not that much and it wouldn't be consistent. My best guess is two possibilities, 1) your endmill is undersize and you didn't apply the correction in the right direction, or 2) your machine calibration is not correct. I'm going to say #2 is the culprit.