[IN-WondeR]

The fact that you tried doing a cut where you left a tool offset at 0.5mm to do a finish cut should tell you a lot.
It is your tool deflecting more than your machine.

I have an all steel built and welded machine, and if I do all my cuts without leaving the offset (with a 1/8") cutter, then i to get a difference from the design, to the finished part.
But if I leave the offset when going into the material, and do the finish pass at the end, the size and sides are pretty much perfect with a difference of only 0.06mm in difference. Still with the same single flute cutter.

So instead of beginning to change a whole lot on your machine, think of the way you machine your parts instead. It might be better to do it this way, rather than beginning to change the entire setup of your machine.

On that note.

I still think your hangout from your z axis backplate is too long. Even though your plate is 20mm thick, there will be cause for deflection in that plate.

I do believe the 40x80 profiles and 40x160 profile should be good enough.

When you do your finish pass, do it at half the speed your are doing your initial passes, that way you will do a precise finish pass, which theoretically should be more or less perfect.

[kostas1]

The fact that you tried doing a cut where you left a tool offset at 0.5mm to do a finish cut should tell you a lot.
It is your tool deflecting more than your machine.

I have an all steel built and welded machine, and if I do all my cuts without leaving the offset (with a 1/8") cutter, then i to get a difference from the design, to the finished part.
But if I leave the offset when going into the material, and do the finish pass at the end, the size and sides are pretty much perfect with a difference of only 0.06mm in difference. Still with the same single flute cutter.

So instead of beginning to change a whole lot on your machine, think of the way you machine your parts instead. It might be better to do it this way, rather than beginning to change the entire setup of your machine.

On that note.

I still think your hangout from your z axis backplate is too long. Even though your plate is 20mm thick, there will be cause for deflection in that plate.

I do believe the 40x80 profiles and 40x160 profile should be good enough.

When you do your finish pass, do it at half the speed your are doing your initial passes, that way you will do a precise finish pass, which theoretically should be more or less perfect.

Thanks for the reply,
I think that my machine is deflecting more than my tool, because I set my tool, feeds and speeds according to GWizard's no-tough calculations.

I don't want to start replacing the cnc parts (no time and money), but I asked if these steps could improve cnc's stiffnes.

Regarding the backplate deflection you mentioned, maybe the part that causes more deflection is the little alu profiles 20x20mm (mounted with T-nuts) behind the alu backplate.'

Also, by the way, does anyone know if the setting for allowing some material for the finish pass is the 'Allowance offset' in Vectric Aspire?Please verify.

Thanks.

[IN-WondeR]

The setting you are looking for is "allowance offset"
This will for the first profile cut, leave 0.5mm material, then you create another profile cut, that removes the last of the material.

And you can always do your finish pass in one cut, just changing how many passes you want it to do the finish pass in.

The 20x20mm profiles you have mounted, how many t-nuts are they attached with??

I think we are talking about two different things, when we say z axis backplate. I mean the moving plate on your z axis.

[kostas1]

The setting you are looking for is "allowance offset"
This will for the first profile cut, leave 0.5mm material, then you create another profile cut, that removes the last of the material.

And you can always do your finish pass in one cut, just changing how many passes you want it to do the finish pass in.

The 20x20mm profiles you have mounted, how many t-nuts are they attached with??

I think we are talking about two different things, when we say z axis backplate. I mean the moving plate on your z axis.

There are 6 T-Nuts per profile.
I think we are talking about the same plate. I mean the #2 in the image attached.
Thanks.

[IN-WondeR]

Yes, then we are talking about the same plate... The part of it that is not supported by the bearings, could be a source of deflection.
And your spindle is hanging on that area only,

What diameter tool are you using??

[kostas1]

Yes, then we are talking about the same plate... The part of it that is not supported by the bearings, could be a source of deflection.
And your spindle is hanging on that area only,

What diameter tool are you using??

All the tests performed with 3.175mm 2 flute spiral carbide bit. stickout 24mm, 3mm per pass, 6 passes, 18mm thick wood material.

[IN-WondeR]

a 3.175mm tool will easily bend. And if they are cheap chinese ones, they will probably bend easier...

But if you do it the way I wrote, I will guarantee you nearby perfect cuts everytime...

[kostas1]

a 3.175mm tool will easily bend. And if they are cheap chinese ones, they will probably bend easier...

But if you do it the way I wrote, I will guarantee you nearby perfect cuts everytime...

Yeah, I am using chinese bits 3.175mm, 24mm stickout. Where can I find some decent bits from the ebay? What I am using now is carbide with extra band (at least this is what he says) THe supplier's nickname is 'dobest tools'

[mmoe]

I would recommend Vortex tools for router bits. They are some of the best I've used and they aren't that much more in cost once you factor in longevity. Cheap bits will have an adverse impact on the quality of the cut for sure.

I'm cutting a bunch of solid body guitars (strat style) and the results I get for pockets etc. are as close to perfect as you could hope for. I always leave a .5mm allowance for a clean-up pass and I always climb mill, even though for most wood working applications I prefer to conventional mill. When climb milling in wood, especially with smaller diameter bits like 1/8", I find you have to drop your feedrates from the recommended a little, so the calculator is a little less useful than first hand experience. I run 1/4" bits at 15,000 rpms and 1200mm/min for the clean up pass, while nearly double that at 2000mm/min for roughing. In 1/8" bits, I run them at 1500mm/min at 1/4" deep for roughing passes, followed by 1000mm/min for cleanup passes up to 1/2". I'm not sure where you got a 1" long flute, but that's just too long for a 1/8" bit in my opinion. If you need 1" of flute, you should go up to a 1/4" bit and then clean the corners out by hand or by a "rest machining" or "pencil trace" to sharpen only the corners up with the 1/8" bit afterwards.

Also, it looks like you don't have any sort of lead in? I don't know how specific you can be with Vectric, but I like to do what's called a tangental lead in with a 45 degree entry. In this style, the bit moves for approx. 2mm or 3mm at a 45 degree angle from the part edge, then moves around a 3mm-6mm arc until it becomes tangent to the part edge. I then overlap the exit so that there isn't that little nub left at the entry/exit point, usually a 3mm overlap unless the specific pocket is too small. The larger the lead in arc radius and the better the overlap, the more minimal the entry/exit will be, so I go as big as I can within the constraints of the geometry. Using this lead-in and lead out strategy, you can't identify where the start and stop of the cut was, even by feel. I would also try to start/end in the middle of a straight section rather than right where a straight line meets up with an arc, but that's a smaller issue than getting the overlap and entry arc in the end (the overlap would just follow the arc in this case until it exits).

[kostas1]

I would recommend Vortex tools for router bits. They are some of the best I've used and they aren't that much more in cost once you factor in longevity. Cheap bits will have an adverse impact on the quality of the cut for sure.

I'm cutting a bunch of solid body guitars (strat style) and the results I get for pockets etc. are as close to perfect as you could hope for. I always leave a .5mm allowance for a clean-up pass and I always climb mill, even though for most wood working applications I prefer to conventional mill. When climb milling in wood, especially with smaller diameter bits like 1/8", I find you have to drop your feedrates from the recommended a little, so the calculator is a little less useful than first hand experience. I run 1/4" bits at 15,000 rpms and 1200mm/min for the clean up pass, while nearly double that at 2000mm/min for roughing. In 1/8" bits, I run them at 1500mm/min at 1/4" deep for roughing passes, followed by 1000mm/min for cleanup passes up to 1/2". I'm not sure where you got a 1" long flute, but that's just too long for a 1/8" bit in my opinion. If you need 1" of flute, you should go up to a 1/4" bit and then clean the corners out by hand or by a "rest machining" or "pencil trace" to sharpen only the corners up with the 1/8" bit afterwards.

Also, it looks like you don't have any sort of lead in? I don't know how specific you can be with Vectric, but I like to do what's called a tangental lead in with a 45 degree entry. In this style, the bit moves for approx. 2mm or 3mm at a 45 degree angle from the part edge, then moves around a 3mm-6mm arc until it becomes tangent to the part edge. I then overlap the exit so that there isn't that little nub left at the entry/exit point, usually a 3mm overlap unless the specific pocket is too small. The larger the lead in arc radius and the better the overlap, the more minimal the entry/exit will be, so I go as big as I can within the constraints of the geometry. Using this lead-in and lead out strategy, you can't identify where the start and stop of the cut was, even by feel. I would also try to start/end in the middle of a straight section rather than right where a straight line meets up with an arc, but that's a smaller issue than getting the overlap and entry arc in the end (the overlap would just follow the arc in this case until it exits).

Thanks for the info mmoe,
Indeed, I need to try with some better cutters instead of the chinese and make some test cuts again. However, I noticed that the biggest step in quality improvement was to just use the allowance offset and then do a finish pass. I tested just once the climb milling while roughing but the result was not encouraging. However, I haven't try climb milling while finishing because convetional milling gave me what I needed.

Also, yes, I do not use the lead in, thanks for reminding this to me. Aspire supports this feature (please check the attached image)

[mmoe]

If it were me, I'd check the "Do lead out" box and see if the "Overcut Distance" give you some overlap between the lead in and the lead out. If possible, make it 2 or 3 mm and you'll find your entry points should be invisible. If not, you have some mechanical issues that may need worked out.

Here's a photo (tremolo pocket) where there are three lead ins/lead outs (one at each level) shown in the image, roughly in the center of each wall/level. You'll see that you can't make them out at all. There is a slight step on one vertical wall where the second, lower pass was a much heavier cleanup than the first one (about .002" using a feeler gauge), but it's otherwise a very clean pocket. The wood is extremely old growth Douglas Fir, which is similar in hardness to genuine Mahogany in my estimation. I've used it for many guitars over the years and it's one of my favorites to work with. On average, there are around 45 years per inch across this guitar body, which was made as a 4 piece (45 early wood and 45 late wood rings). In the past, I had trouble rounding over the edges as it really likes to chip out, but as you can see from the neck pocket, I can now produce a chip free roundover right to a knife edge using a ballend mill, which can also trace around the 3d contours perfectly. CNC routers have really changed the level of precision and finish quality for guitar makers in my opinion, but like all tools it takes a bit of time to get your methods working to their fullest potential.

For full disclosure, my machine is not really a hobby machine, so I can't really relate much to machine deflections and don't have much knowledge about how significant or insignificant it should be. My machine weighs in at around 8000lbs (over 3500 kg) and can produce two guitar bodies simultaneously using two 10hp heads. The feeds/speed I suggest are more of an ideal machine speed, so if you have some degree of deflection beyond the cutters, you may have to go a little slower or take lighter passes. But hopefully they still give you a starting point of what should work with quality cutters.

[kostas1]

If it were me, I'd check the "Do lead out" box and see if the "Overcut Distance" give you some overlap between the lead in and the lead out. If possible, make it 2 or 3 mm and you'll find your entry points should be invisible. If not, you have some mechanical issues that may need worked out.

Here's a photo (tremolo pocket) where there are three lead ins/lead outs (one at each level) shown in the image, roughly in the center of each wall/level. You'll see that you can't make them out at all. There is a slight step on one vertical wall where the second, lower pass was a much heavier cleanup than the first one (about .002" using a feeler gauge), but it's otherwise a very clean pocket. The wood is extremely old growth Douglas Fir, which is similar in hardness to genuine Mahogany in my estimation. I've used it for many guitars over the years and it's one of my favorites to work with. On average, there are around 45 years per inch across this guitar body, which was made as a 4 piece (45 early wood and 45 late wood rings). In the past, I had trouble rounding over the edges as it really likes to chip out, but as you can see from the neck pocket, I can now produce a chip free roundover right to a knife edge using a ballend mill, which can also trace around the 3d contours perfectly. CNC routers have really changed the level of precision and finish quality for guitar makers in my opinion, but like all tools it takes a bit of time to get your methods working to their fullest potential.

For full disclosure, my machine is not really a hobby machine, so I can't really relate much to machine deflections and don't have much knowledge about how significant or insignificant it should be. My machine weighs in at around 8000lbs (over 3500 kg) and can produce two guitar bodies simultaneously using two 10hp heads. The feeds/speed I suggest are more of an ideal machine speed, so if you have some degree of deflection beyond the cutters, you may have to go a little slower or take lighter passes. But hopefully they still give you a starting point of what should work with quality cutters.

Thank you very much for this info my friend,
what do you do when you add tabs on your profile toolpaths? Is there any way to avoid cutting marks before and right after the tab?

[mmoe]

I think you can make the tab start/end have a ramp, so probably the best you can do is to keep the ramp angle shallow. I don't use tabs very often and prefer to use either a vacuum fixture (if I'm doing the same part over and over) or a quality double stick tape for those one-off projects or prototypes. The double stick tape I use is strong enough that I have machined 2" thick aluminum bar stock without any problems with movement, so anything in wood is very easily held that way. It's basically just a paper-based masking tape with sticky on both sides. This provides a thin tape with very good adhesion, but it comes off without damaging the part as well, though usually I have to pry the part off with a putty knife because it's held on so well.

I believe the tape I use is number 592 at the link below, so if you find something similar, it should work well:
Double-Coated Tape / Double-Sided Tape from IPG

[kostas1]

Hi again guys,
so, this past weekend, I tried the 3d tabs and also the roughing cut and then the 0.5mm finish cut, both convetionally. The climb cut finish gave me not clean and accurate objects and I went back to conventional cut.

However, please take a look at the attached images to explain my issue:

When cutting the top part of the design (the 5 arcs) from right to left as the arrow indicates, the machine passed from the first 2 arcs inside corners more quickly than the rest 3 arc corners and this resulted to a more grooved corners. I hope you can make out the diferrence in the corners(green areas) between the right arcs and the left arcs. The left arcs corners are sharper than the right's ones but also with a little groove.

The finish speed was set to 1300mm/min and rough speed to 2300 mm/min. I know that in conventional milling the router bit tends to be pushed into the material, but I also need to mention that I have the mach3 setting 'Stop CV on angles > ' to 15. With this setting shouldn't the cutter passed in the same speed both left and right arc inside corners? As we can notice, these corners are greater than 15 degrees so it should pass the same fast in both of them.

What might be wrong?
Is there any deflection again that emerged?

Thanks.

[kostas1]

a 3.175mm tool will easily bend. And if they are cheap chinese ones, they will probably bend easier...

But if you do it the way I wrote, I will guarantee you nearby perfect cuts everytime...

Hi friend,
I tried your solution, where I made 6 passes of 3mm depth with 3.175mm chinese tool (bought from 'dobesttools' in ebay) and then a finish cut of 0.5mm width and I have variations in the size. Almost the 2/3 number of pieces are good but the rest are not satisfactory. Please take a look at the attached image. The left rectangle area's width is 0.5mm bigger than this of right rectangle.

Any suggestions would be very helpful.
Thanks

[ger21]

Your pics at the top of the headstock look like you have a considerable amount of play somewhere.
Are you cutting the slots and the headtock at the same time? Is everything cut in the same direction. I can't see how one slot is shifted .5mm. Is the CAD file correct?

[kostas1]

Your pics at the top of the headstock look like you have a considerable amount of play somewhere.
Are you cutting the slots and the headtock at the same time? Is everything cut in the same direction. I can't see how one slot is shifted .5mm. Is the CAD file correct?

Hi Gerry, if you are referring to my post #35, then I firstly cut all the slots from several holded down parts and then I cut all the profiles from these. Everything in the same direction. Also slots' width is nearly perfect, according to cad file..
The aspire file is correct. I checked too many times.

Thanks.

[kostas1]

What I can think of the parts' size being varied from part to part is the grain in material. Maybe the grain in some places is tougher and the chinese bit or z axis deflects more. I have cut 60 same parts and 40 of them are satisfactory but the other 20 vary from 0.2-0.5mm. However, both roughing (6 passes) and finish(1 full depth pass) cuts were made with conventional method.
What I haven't tried yet is rough climb cut in 6 passes and then 1 full depth pass of finish conventional cut.

Also, as some of you guys said, I now also think that the z axis deflects but not sure how to fix this

[ger21]

Somewhere earlier you measured quite a bit of deflection. I think you really need to find the source of this and try to eliminate it. I doubt that the bits are the cause of your issues.

[kostas1]

Somewhere earlier you measured quite a bit of deflection. I think you really need to find the source of this and try to eliminate it. I doubt that the bits are the cause of your issues.

Yes I measured the deflection by applying force with my 1,2,3,4 fingers and one hand. It is described in my post #20. However, I am not sure if this is in the right way to do so, but it is very possible that the reason is z axis deflection. Now how could I locate and fix this deflection? Maybe, as I ve told, it is the two 20x20mm aluminium profiles that hold the z axis rails.