verhoevenc Posted August 1, 2017 Report Share Posted August 1, 2017 So although I feel I'm getting a pretty good handle on the CNC stuff lately there is one thing that continues to remain elusive to me: really clean body route edge. First I'll describe what I'm doing. Then what I've seen others doing and what I believe are the other options. Ok. So I started off using a 2-flute spiral upcut (for chip clearance) and that seemed to work ok. However in order to get the chipload where it needed to be I was running my machine at a faster feed rate than I wanted to; 3IPS at 12,000RPM. My machine's max cut is 4IPS and after I had it lose some steps going at 3IPS I was told on a Shopbot forum not to push that boundary. Plus, it wasn't the cleanest cut so I was happy to try other stuff. I went out and got a spiral O-flute single-flute 1/4" bit instead. The flute decrease and chipload recommendation brought my suggested feed down to 1.33IPS which I felt better about. This made for greatly improved chip clearance (bigger flute and slower speed in guessing) and I saw none of the lost steps issues I saw before. Whether that's due to speed or improved chip clearance I do not know. However, my surface quality didn't appear to go up much. I even went about doing my initial channel .015" offset and then coming back in and 'onion skinning' conventional cut that last little bit. Alas, still some bad spots as you can see in the pic below of a student body that used exactly that method. The body was flipped half way through and you can see that the bit left rough patches in the same section, as per rotation vs grain direction, on both sides. Heres what I think is happening. A 1/4" bit isn't THE most rigid thing in the world. When you tell it to go into a 1/4" hole, clear chips while it's at it, and cut cleanly, it's telling me that that's too much to ask. I'm guessing there's too much binding going on, or friction, or heat, or something in that small channel. The .015" onion skin pass was then not thick enough to remove all the chatter? What I've seen others do, or what my head thinks might be an improvement: 1- do the pass where the bit is the same diameter as the whole channel a full 1/16" offset out. Come back and take off the last 1/16" in a second round. This gives the bit breathing room and also allows you to vacuum out all the chips from round 1 to help clear the channel between paths. 2- Leave indexing pins at a couple locations so you can re-locate the body later. Then mill an 1/8" deep body outline into the blank. Pull it off the CNC and bandsaw it really close the that line. Re-attach to the CNC and route the outline full depth. This would mean you're edge routing, not even routing a channel. 3- move to a 1/2" bit that's more rigid. I don't particularly want to do this as this then requires my blanks to be larger to continue to accommodate the placement of my indexing pins. Seems like wood waste. Also, I've never used a 1/2" bit on my Shopbot Desktop despite it coming with a 1/2" collet. Not sure about the machine's performance with one ATM. It could also be that I'm doing something else wrong... happy for insight that saves me experimentation time. Chris Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 1, 2017 Report Share Posted August 1, 2017 Chris, I apologize if I have asked this before,my old mind has slept a few times since. My first question is what is the spindle or router being used and what is the HP rating? 1/2" bits will definitely help. That being said, what type of collet are you using? If you are running the standard collet on say a Porter cable router then this is going to give you more runout and increase chatter. What are the bits /endmills designed for? Are they for wood router bits or metal cutting endmills and what type of metal are they designed for? Are they TIN or something similar coated or not? Just trying to get a better understanding of what is happening? As you know any endgrain will give less than a smooth finish but it can be mitigated to a better finish than what you are getting based on the pictures. One more thing, try using some red oak as a test wood for this. It is much less expensive and very stringy. It will help you with the process of dialing it in. Mike Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted August 1, 2017 Author Report Share Posted August 1, 2017 Spindle is 1HP and the standard Shopbot Desktop offering in the spindle space. Bits aren't coated. Onsrud carbide stuff, this one in particular is the 63-727. Believe the collet is an ER20...? Chris 1 Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 2, 2017 Report Share Posted August 2, 2017 19 hours ago, verhoevenc said: Spindle is 1HP and the standard Shopbot Desktop offering in the spindle space. Bits aren't coated. Onsrud carbide stuff, this one in particular is the 63-727. Believe the collet is an ER20...? Chris Okay cool , check your spindle run_out to make sure it is in spec. Most spindles should be within 0.005mm or 0.0002" at 1" from collet. If it were me I would try this end-mill. http://www.shars.com/products/cutting/end-mills/1-2-x-1-2-4-flute-long-length-m42-8-premium-cobalt-single-end-end-mills-1 Spindle RPM about 12K to 13k DOC 50%d 70 to 80IPM use this as a base line try on Oak and find the sweet spot. MK Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 2, 2017 Report Share Posted August 2, 2017 On 8/1/2017 at 9:49 AM, verhoevenc said: >snip< Heres what I think is happening. A 1/4" bit isn't THE most rigid thing in the world. When you tell it to go into a 1/4" hole, clear chips while it's at it, and cut cleanly, it's telling me that that's too much to ask. I'm guessing there's too much binding going on, or friction, or heat, or something in that small channel. >snip< Chris this sounds like it could be a tramming issue? Mike Quote Link to comment Share on other sites More sharing options...
curtisa Posted August 2, 2017 Report Share Posted August 2, 2017 Have you tried changing the toolpath direction? In the cutaway 'hollows' for example, it might be worth seeing what happens if you divide each curve up into two separate toolpaths - one that goes in a clockwise direction and one in an anti-clockwise direction, radiating away from the centre of the cutaway.. Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted August 3, 2017 Author Report Share Posted August 3, 2017 @MiKro are those numbers correct...?! A 4-flute bit for wood? At an effective chipload of .00145 (tiny!). This seems to go against most things I thought I'd learned about chipload. Agree might be 'tramming.' @curtisa I'm sure that's likely help as if you switch direction it leaves the tesrout on the other side. So yes it could be strategically avoided. But what a PITA. I don't see anyone else having to do that so there must be an easier way? Chris Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 3, 2017 Report Share Posted August 3, 2017 Chris the numbers are a start point, use what you think will work for your machine. Remember I use these with a Router and PWM speed control at low rpms. A spindle will give you different results I'm sure? So follow your gut and adjust. When I cut things I am not concerned about time, more about quality. One more thing don't get to caught up in the chipload vs IPS/IPM, go with what works. That comes with trial and error. Mike Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted August 20, 2017 Author Report Share Posted August 20, 2017 No kidding a starting point! OK, so I ran some tests... and by that I mean a lot of tests. Basically draw a ton of lines and cut them at every possible feed/speed combo that I could (within reason for jumps in IPS and RPM). All of this was done with an Onsrud 65-000 (single flute upcut O-flute) endmill. According to Onsrud's chipload chart (https://www.onsrud.com/files/pdf/2012 LMT Onsrud Production Cutting Tools Hard Wood.pdf) this bit has a recommended chipload in hardwood of .004-.006 With this in mind I set up the following 3" lines, .2" deep, single pass: 9000RPM 1IPS= .0067 <- best of the 9000RPM tests 2IPS= .013 3IPS= .02 4IPS (my machine's max cut speed)= .026 12000RPM 1IPS= .005 <- best of the 12000RPM tests 2IPS= .01 3IPS= .015 4IPS= .02 15000RPM 1IPS= .004 <- best of the 15000RPM test 2IPS= .008 3IPS= .012 4IPS-.016 18000RPM 1IPS= .003 <- best of all the tests so far 2IPS= .006 3IPS= .01 4IPS= .013 Looking at the channels and judging them for cleanliness I found that .003 chipload in the 18000RPM bracket was the cleanest. My definition of "clean" wasn't just cut marks being left by the bit, but more importantly a lack of tearout as all the tests purposefully cut across end grain, which is the only real place I'm having cleanliness issues when cutting out guitars. It was surprising to see that the lowest value was the winner; especially since it was out of Onsrud's recommended range. Note, only two other values were within their range though; .004 and .005 With this new knowledge I went back and calculated chiploads of .001-.004 in .001 increments, all at 12000RPM (as this is what I've been told is ideal for wood). The results of these tests are: .001 as .2IPS .002 as .4IPS <- winner .003 as .6IPS .004 as .8IPS Although .001 was very nice and clean, I could see that the "chips" coming off this cut were very small. Seeing as .002 was just as clean, had nicer chips, and is twice as fast, this was the winner. .003 and .004 both started to show signs of tearout of the end grain. In conclusion the winning chipload for this bit is not only outside of the manufacturer's recommended range, but also a mere 50% of the recommended range's lower bound?! Can this be right? I'm going to do some more extensive tests with this chipload value... but I find it hard to believe that the manufacturer recommendations are so off? Chris PS: The wood used was quartersawn sapele scraps. 1 Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 20, 2017 Report Share Posted August 20, 2017 Funny how that works? Very close to the same chip load calculated for the 4 flute @ 12000rpm. Good for you Chris, I am happy that you are finding what works in real life for you is not just the #s they say they are. My method is a lot less analytical, I just go with what looks and sounds right. LOL!!! Good info there my friend. Mike Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted August 20, 2017 Author Report Share Posted August 20, 2017 Ok, last post on boring tests and numbers for the day; promise. These are the sizes of the chips being produced by the .002 chipload. They eyeball at around .002" thick so that seems logical. This is the shape I did. Grain runs left to right. End grain side 1 is incredibly smooth. End grain size two has some very minor fuzziness... but still nothing compared to what I've been dealing with before (was previously running this bit at 1.33IPS @ 12k... so a chipload of .00665). Here's the side grain. Again nice. Other problem I still seem to have is chunks of wood being lost in sections of extremely short grain (think the corners of headstocks...). This I'll still have to run tests to alleviate. All in all I think I have found my desired chipload for this one bit (hahahaha). I'm also fairly confident that if I were to run these cuts with a .015" offset and then come back and do a full-depth onion-skin pass to remove that last bit that I would be left with stellar results. I wish I'd have thought to test that while everything was still on the table... Chris Quote Link to comment Share on other sites More sharing options...
MiKro Posted August 20, 2017 Report Share Posted August 20, 2017 Very Nice Chris. One thing though, how much heat gain will your spindle have from lowering the RPM? I will be using a spindle once all is said and done and just testing the spindle I see a greater amount of heat from it @12K vs 18K, Just something to consider in this. Like I said your setup is different than mine was , now I may be closer to yours and will be relearning. MK Quote Link to comment Share on other sites More sharing options...
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.