@Retiree With respect, I can understand why you are perplexed. I completely agree that your problem is being caused by the toolpaths you are creating. Itās not an inherent fault of the router, except for the fact that we all need to take into account that we using a trim router for a purpose for which it was never designed. We can accommodate that āweaknessā by watching feeds, speeds, depths of cut, stepover, etc. But we cannot eliminate it.
I address that by being very conservative with my toolpath settings. So far, that approach has held me in good stead.
If you like, if you are using VCarve, I will look at your .crv file to determine if anything really jumps out. Otherwise, Iām sure that, at some point, you will solve this with the help of other members.
Thanks, Grant - you got me thinking - always a good thingā¦ agree with your characterization of the router - it is designed as a trim router, not a CNC spindle, so always limitations, as you indicate.
I will try further carving with a significantly reduced F&S and see what happens. The obvious question is how āconservativeā to go. At some point, I expect there will be no slippage.
Appreciate your offer to look at my file. Letās wait until after I do some more experimentationā¦
@Retiree There is no hurry from my end. My offer is open. I may have some thoughts on how to increase your chances of success, but I would want to see the file before offering them up.
As to what is āconservative enoughā, Iām sure that you understand that there is no easy answer. I have been roundly criticized by people far more knowledgeable than me about feeds, speeds and chip load. In their expert opinions, I should be pushing my LM and the Makita router more. I have long ago given up arguing my case. I donāt dispute their superior knowledge at all. However, I fall back on the fact that my methods provide the results that I am looking for. In your experimentation, I am sure that you will find that there is more than one way to skin this cat. I am also sure that you will find a way that works for you. That confidence comes from the fact that thousands of others have succeeded using the same equipment that you are using. Good luck.
Eureka! Got a 45 min cut with no slippage! (kept clothes on). I am very new at this, so learning, experimentingā¦amazing how many parameters one should consider and trade off, and now add one more - the holding power of a Makita router collet. There is always a limit for everything. Detail: Sienci chart indicates 150 ipm for this TBN mill for carving/detailing for hardwood, so trying to be āconservativeā, I started at 130, then at 100 - slippage on both. Today, ran at 65 and SUCCESS! I have no doubt that I am creating flour instead of chips in some areas, however, the prime objective is to get the result I want. Downside, of course, is that it will take much much longer to cut a project. Am impressed with GSender 1.5 capabilities to stop/restart a job as well as changing feed rate on the fly.
Since I have ruined this project and still have more cutting to go to completion, I have one more area to experiment with. I indicated earlier that I bought a router from Carbide3D with an ER11 collet. I plan to install it, and then try the higher F&S.
Will KYP.
Many thanks to all of you for providing ideas and suggestions. I am grateful we have this forum.
@Retiree Thatās very good to hear. If you would agree, I would still like to see your file and toolpaths. Going forward, you should not need to go that slow. I run my .06 tapered ball nose on finishing passes at 150ipm with no issues at all.
I hope I havenāt made you feel that way too much. Was never my intent to make anyone just give up. Iām always trying to explain the why in a way that hopefully matches the limits of the available systems. If thereās a reason that wonāt work I want to know. Iām not advocating to push either āharderā. Most of what I try to get across is where to make the compromise to get better results.
Completely get that. At the end of the day you go with what works.
Both to this and to gwilkiās post prior. Yes, you can get this down enough to reduce engagement time and force to keep inside limits. If you HAVE to make that sacrifice, so be it. But, I donāt think you have to.
Iāll try to break this down better than I have before. You are dealing with 2 issues. Force of the cut, and engagement time of each flute of the cutter. Since Iām trying to keep this simple. Iāll put this here. The below is for a given tool and material. Changing those is another variable but Iām not going to interject into the flow of the below to point it out each time.
The force of the cut is functionally how much material you are removing and how fast. So stepover, chipload (feed), and pass depth for any given material produces a force that everything has to resists. Any increase or decrease in those results in a relatively proportional change in force. That force is what the machine, material your cutting, tool, and Iāll throw in here collet has to resist.
A simple version of engagement time is for a given force (above) how long is a single flute creating a force. Or an even simpler one, how long is a flute ātouchingā material in rotation. When not dealing of a straight flute cutter this is more or less increased by the cutting depth.
Combining the above is why I advocate for pushing the machine and router āharderā, while reducing the pass depth. Itās not actually harder on the machine or tool, gives a better chip (cut), and reduces the engagement time.
In this example you have even more advantage reducing the pass depth. As the tool is tapered and when entering a section that the roughing tool canāt reach into you are functionally increasing the āstepoverā in addition to the depth.
So if you havenāt yet. Iād also try the āsimpleā multi-pass cut on this. Just take your Z and when setting your Z zero fake a partial plunge. Then you can increment your zero to finish the actual cut you need. E.g. of the total Z depth is -0.5, set your Z zero to instead of 0, -0.25, cut, set zero to 0 cut. That will give you more or less half the force. Although, not in the same directions (X,Y,Z). You could do the same thing in 3 or 4 passes by just dividing the total Z by the number of passes you want and altering you zero.
Hope that makes more sense than the other times Iāve posted similar.
@TDA My comment was not directed at you, John. Nor were they directed at your posts here. Over the course of years, I have received some x-rated emails telling me in no uncertain terms that, not only do I not know what I am talking about and that I am a liar, but that I should simply shut up and blow away. Iām still here.
I carefully read all your posts. I have learned a great deal from them. I have no doubt that will continue in the future.
Also, FWIW, Retiree lives close by. I have his .crv file and I believe that there is a simple way to resolve his issues. Time will tell if Iām right.
TDA. Your explanation makes sense to me. From a practical perspective, I see two choices to achieve the result I want: either reduce feed rate by a factor of two or make two passes at full feed rate. (I agree with the nuance of two passes providing an additional stepover effect, but wonder how large a factor this is). Both choices leave me with the issue of a huge amount of cutting time, and of course, no guarantee that the DOC will be reliably stable. A new project (large) I am considering, is estimated at 34 hours cutting time for the Finishing cut at half feed rate. I guess I better check my camping gearā¦
gwilki has kindly offered to check my file and toolpaths. I plan to wait until he has had a chance to do this before trying anything else.
Without seeing your vcarve model, I may be way off baseā¦
Could you break the pocket/roughing/finishing toolpath into multiple toolpaths set up so that each toolpath avoids the problem?
My first (naive?) idea would be to make small offset closed shapes inward from the outer wall, and outward from the inner butterfly, and then create a series of crafted āsafeā toolpaths that mimic the different bit and F&S choices that Vectric makes for you when setting up an āautomaticā pocket-with-roughing-passes:
(rough drawing of what Iām thinking, with the offsets in red)
Toolpath 1: rough out the black line pocket between the butterfly and walls - From your comments above, this doesnāt seem to be the source of your problem
Toolpath 2: finish the inner red line pocket - will take a long time with a small TRO bit, but should never run into the āfull wall engagementā bit slip problem because of the red offset distance
Toolpath 3: a multi-pass āinside the outer black lineā profile finishing pass with pass depth (or feedā¦) set to eliminate the slip problem
Toolpath 4: a multi-pass āoutside the inner butterfly black outlineā finishing pass ā¦ dittoā¦
gwilki and I met - many thanks for spending the time with me and for sharing your experience. I learned much.
We agreed that the TBN mill IS slipping on the cut and model I have been doing (note: I have had no issues with any other mill). The evidence points to the abrupt contact of the flutes with the 1/2ā vertical āwallā of my model, creating a sudden downforce on every pass, which exceeds the holding power of the Makita collet. Solution is to either reduce the feed or take several passes, as per previous advice.
My simplistic approach has been to do a rough cut, then a finishing cut. Gwilki suggested that I pocket the flat background first, then run a straight 1/8ā ballnose as a rough cut over the model, and then the finishing TBN. Will definitely reduce total cutting time, and the sense (hope?) is that this should soften the vertical āwallā of the model. While intriguing, I do not plan to repeat this āexperimentā, but do plan to take this approach into account where possible on the next projects.
My next step is to replace the Makita router with one I bought from Carbide3D - it has an ER11 collet.
Earlier in this thread there was a sidebar on ordering things from the US to be delivered in Canada. I indicated that Carbide3D seems to have a secret sauce to achieve this without brokerage, taxes, etc.. I was wrong.
4 weeks after I received the shipment, I received a letter (yes, snail mail) from Fedex indicating that they had paid all kinds of fees āon my behalfā and now I owe them some $ās. I have indicated my complete displeasure with their business practices. UPS makes you pay the fees on delivery of package. No one seems willing to provide an estimate of fees in advance so that the customer can make an informed decision.
Outcome is that these packages (all under $100 Cdn) wind up costing close to double the product cost. Amazon.ca looks better every day
Re: the courier ābrokerageā fees, this is a long-standing issue. I am not surprised at your outcome - unfortunately. From experience, I can tell you that if you do not pay Fedex, they will be very, very aggressive at pursuing it. As to not providing you with an estimate in advance, again from experience, I can tell you that the shipper does not know this information and the courier will not provide it to them. There are services that the shipper can choose which include all import fees, but they are much more expensive than the normal shipping options.
