Noob question, full disclosure this is my first experience with a CNC type machine and by extension this is far more time I have spent using a router than all of my previous years of age combined. So here is my question: how long do router bits last? how do i tell when it needs to be replaced? I bought a couple 1/4" straight router bits from Home Depot when I purchased the Ridgid 2202R just so that I had everything needed to assemble my Maslow when it arrived. I have yet to finish cutting all the pieces for the “final” frame. I’m about 30% through the “allparts.svg” file , I didnt realize it was going to take so long (hours so far) but it makes sense since its going through multiple passes on 3/4 plywood takes time at 10mm increments. Then I began to wonder is the bit getting dull? Should it last through the whole build process of the Maslow assembly? Multiple times for a second or third maslow frame (each using a new 3/4" plywood sheet) ?
I also ordered a couple of the more economical bits now being offered on the Maslow site, but same questions apply how long should they last and how do i tell when they need to be replaced? I realize it depends on the material being cut and the thickness, but to keep the comparisons based on my limited experience, please respond with “it should be able to cut “X” number of 3/4” plywood sheets. or # maslow final frame parts, as this is the only comparison I can grasp at this point with my limited experience. Or I am totally off base? I hope it all makes sense. Please advise. So far I am super excited to start creating new things!!! Thanks for this wonderful concept brought to life.
I don’t think anyone can give you a fixed number. But there are things you can look out for:
Does it look damaged?
Does it look scorched (you might have your spindle speed too high)
Does the resulting cut look bad have lots of splinters or looks rough
Does the machine sound different than when you had a new bit
Is the sled tilting because it can’t cut the material as fast as it used to
You just have to experiment, some people tolerate more worn bits than others. If you think it has passed its expiration, take it out and put a new one in. Then check to see if the resulting performance is noticeably better. If it isn’t maybe hold on to that first bit for use again later.
If everything is working well, you can cut all of the frame pieces and still have a good bit. But if you are like me, you will have accidentally set the spindle speed too high (I wasn’t really thinking and did it all at 18k). When I was done, my bit was noticeably discolored and it had a hard time keeping up with my normal feed rates.
I notice a couple spots that it scorched , I have it set around 15-18k Similar to your settings. I didnt see any guidance in the assembly Wiki so I went with a half way setting on the dial/unit.
Not sure, compared to what? I guess need more experience to get an eye for such nuances. This will come in time i suppose.
[quote=“krkeegan, post:2, topic:274”]
Does the machine sound different than when you had a new bit
[/quote] Will try it out.
Yes, I could see the sled tilt as it would start each new cut/pass, this is what made me consider the duration of the router bits. I presume I need to increase the speed of the spindle but after your initial response and “scorched” remark it should be slower right? I guess that might be another topic but what would be a nominal setting for the Ridgid 2202R and 1/4" bit on 3/4" plywood? (using feed settings example from the wiki) again is it more a personal trial and error to dial it in? I am sure other newbs will have similar questions when going through the assembly guide…
If you check some of the woodworking sites, it is also possible to sharpen or ‘rework’ bits. Normally it isn’t worth the effort. It takes some time, and you might need to adjust your g-code because the bits could be a slightly smaller diameter after processing. As always YMMV.
Just got my kit today in the mail. Hopefully I will be building soon.
I have backed way down to 10k rpm, at 35 ipm, and around .2 inch depth. There are numerous “chip load” calculators out there, just search google. These settings are still below an ideal chip load. Ideally you would want a faster ipm or a slower rpm. Also I think you generally want depth at the radius of the bit. But again, since I am well under the chip load I increased the depth slightly to try and compensate. This is all still experimental for all of us, so there are no hard and fast rules.
But one thing that is a bit counter-intuitive, is that you need larger chips to carry the heat away from the cutter head. If the chips are too small, they don’t remove much heat and the bit can overheat.
Thank you for your very helpful and informative responses. In just my first post I feel I have learned a great deal along with my tangential searching. I feel more confident now in my work and this device purchase as a great investment. Looking forward to participating more in this venture with all of you.
I’m just beginning a build, and have no previous CNC or CAM experience, but approach the subject from a woodworking perspective. I look forward to taking my design ideas in sketch up, and arranging the router workflow, its path, feed rate, depth of cut and therefore number of passes. These variables will be different depending on materials, types of wood, card, etc, I’d imagine.
Ensure an appropriate router cutter path: avoid instances where the router could be allowed to climb-route even with a big sturdy ‘site’ router it can sometimes clip an edge and flick the router significantly. The blade kicking against the workpiece creates a jolt/backlash/kick that can lead to screw-ups and broken bits, so it definitely stresses them!
As a woodworker I’m inclined to make more passes, removing a little each time and keeping the feed rate low, this way keeping bit temperature down and hopefully improving quality of cut. Consideration should be given to grain direction of the wood, any denser knotted areas and changes in the density, many species of lumber are surprisingly variable in their density.
Keep your bits clean. Blade cleaners are available and help remove wood resins and burnt on gunk such as the glues in manufactured and engineered sheet products. Clean them regularly, really regularly if you want a better quality of cut!
Search youtube woodworking channels for specific advice on routing different products, you can whizz through clear pine, but knotted oak panels present a whole different problem!
Correct feeds and speeds are based on the chip load (little tiny piece of material flying off the cutting edge). Each chip needs to have enough mass to remove heat from the cut, as @krkeegan and @dlang described above.
High spindle speeds (rpm) and low feed rates (inches/min or ipm) generates a lot of heat because the chips become tiny and will not have enough mass to remove the heat generated by cutting. This will ultimately result in burning at the extreme and will dull cutting edges very quickly.
Low spindle speeds and high feed rates will result in poor surface finish because the chips are so large that they’re tearing away from the stock. Think of this like biting off more than you can chew. Ultimately, the router will bog down in this case because it just can’t remove material fast enough (although I doubt this is a common problem with Maslow given the current max feed rate of 48 ipm).
Tool life is extended by maintaining a high chip load, but this needs to be balanced by a clean surface finish.
Here’s a handy chip load chart that I use a lot at work. Keep in mind this is only a guideline and developed for solid carbide spiral tooling:
I’d keep your depth of cut to 1/2 the tool diameter to start, especially in hard woods or plastics, and then work up from there if you’re comfortable. Soft material like mdf, plywood, or sign making foams can probably tolerate a full diameter per pass, but always test it first.
And as always, if it sounds bad, it’s probably bad.
Make sure you’re using the right cutter for the job, @czimm74. As @dlang said, compression bits are good for cutting all the way through material in a single pass. If you’re only taking .125" steps and cutting 3/4" plywood, I’d use either an upcut or downcut bit depending on the operation:
Upcut bits remove chips in the upward direction, leaving a nice surface finish in the bottom of the cut.
Downcut bits remove chips in the downward direction, leaving a nice clean edge(s) at the top of the cut.
I typically use upcut bits for pocketing operations, and downcut bits for profiling operations. In your case, I’d probably recommend an upcut bit given the small step.
Weren’t upcut bits recommended to keep the sled from lifting up while cutting?
Unlike a gantry machine there isn’t anything to resist the sled’s upward motion other than the weight of the sled, and only the part that’s perpendicular to the cutting surface. Vectorised math gives me a headache these days, but it can’t be very large
Good call, @mooselake. I don’t think the cutting forces would be very large with a shallow depth of cut, but I can definitely see them being large enough to overcome the small portion of the weight that’s normal to the sled, especially if the depth of cut was higher. Still waiting for a machine so I can’t speak from experience just yet, but downcut bits would be a good way to avoid sled lifting. I guess Maslows are primarily used for cutting out 2D shapes right now (profiling ops), which downcut bits are well purposed for.
Gotta change my perspective a little here. Sorry for the poor assumptions.