Improving Dimensional Accuracy

[rob5standingby (Rob)]

Hi! I’ve had my SO5 Pro for about a year now. This is my first CNC machine, but I’ve known CAD for 15 years and I have done a lot of other woodworking and 3D printing over the years.

For the first year I have primarily been making signs with the machine, and I haven’t really needed for parts to be dimensionally accurate.

Today I cut a simple desk stand for a piece of music gear in my home studio using some 3/4” marine grade Baltic birch and the 201 cutter on my machine.

In Carbide Create, I set the dimensions of a piece to a rectangle, 14” by 16”, and used a contour path with the “outside / right” setting. I decided to measure the piece when I finished, and it’s coming out exactly 1/16” short on both the length and width dimensions. It is, however, nice and square, so that’s great!

Anyway, I tried searching the forums but couldn’t find a similar topic so I decided to ask.

What am I doing wrong here? How can I improve these types of cuts? Here’s an image of my project before I removed it from the machine.

Thank you!
Rob

[WillAdams (William Adams (Carbide 3D))]

Are you cutting slots just as narrow as the tool?

Where possible avoid slotting and add geometry and cut as a pocket

Making vacuum hose adapters

While cutting up vacuum extension wands for this is expedient, it’s a bit problematic given that Shop Vac recently filed for bankruptcy, was bought at the last minute, and production hasn’t caught up. I need a receptacle for the Sweepy 2.0 dust fitting — one option would be to purchase one from Woodcraft, but Carbide 3D sells blocks of HDPE: which looks to be just barely big enough for things to fit. Measuring the hose fitting I get a diameter of ~63.5mm — offsetting that twice we arrive at…

and/or

Adding geometry to cut as a pocket with a finishing pass

One technique which is often suggested to avoid slotting is to add geometry around a part which one wishes to cut out and cut as a pocket down to tab depth — here’s one technique for that. In this case, the project is a bevel gauge which will be cut out of 0.0625" (~1.5mm) thick aluminum: [bevelgauge] Due to the narrowness of the angles, an 0.03125" endmill has to be used, so after importing and scaling the file (we will be cutting out one which is 3") we select the perimeter and offset it tw…

and consider leaving a roughing clearance and taking a finishing pass.

Best Bit for full cut through

One which has a cutting flute length equal to or greater than the thickness of the stock — pretty much any tool should work. Big thing is the toolpaths — if cutting out, rather than just cutting a slot: [image] Offset to the outside by endmill diameter plus 10% or so: [image] [image] [image] Then cut as a pocket: [image] down to tab height or the penultimate pass: [image] then move the contour down to below the pocket and start cutting at the bottom of the pocket: [image] and…

Could you post the file you were cutting?

[rob5standingby (Rob)]

Hi Will,

Thank you so much for the reply. I suppose I didn’t know the terminology to be searching for to find those threads, thank you for sharing them.

I think I understand how I’d recreate those techniques that you’ve posted. I was making this little stand piece as sort of a test to see how dimensionally accurate my machine would be if I wanted to cut entire panels for some workshop cabinets in my garage from 2 by 4 pieces of baltic birch ply that I’ve cut down and laminated with formica.

It seems like the pocketing technique would be very time consuming for making large, rectangular panels, but maybe the “roughing clearance” technique that you mentioned would be the most efficient? I know a CNC machine is not the most efficient way to make very large and accurate rectangles from plywood stock, but I thought it would be fun to try

I’ve attached my Carbide Create file for reference. I am also still sort of trying to figure out speeds and feeds for the SO5 – I believe on this project I tried a few of the HDM “hardwood” presets for the marine grade baltic birch, and just dialed back the depth per pass a little bit for my SO5 with the compact router. For almost the first year I used the “Shapeoko” settings until I realized the machine could be pushed substantially faster I am hoping someday there will be a SO5 setting in Carbide Create.

Thanks for all of your help, Will

20240120_AbletonPushStand.c2d (136 KB)

[WillAdams (William Adams (Carbide 3D))]

You are making the outline cut first:

it should be last (work from inside–out), and you are cutting to a depth of 0.742" w/ a tool which is only 0.25" in diameter — that’s almost 3 times the diameter of the tool.

Instead, move the outline cuts to last:

and select the outer geometry:

and offset to the outside by endmill diameter plus 10%:

Apply:

and cut as a pocket:

down to tab height:

which previews as:

If that is not a sufficient improvement in dimension accuracy then we can add further offset geometry and use it to leave a roughing clearance at the pocket stage.

[rob5standingby (Rob)]

@WillAdams

it should be last (work from inside–out), and you are cutting to a depth of 0.742" w/ a tool which is only 0.25" in diameter — that’s almost 3 times the diameter of the tool.

Thanks so much for the in-depth response, Will! It looks like the pocketing method adds significant time to the total cut of the project (42 minutes versus 132 minutes), but I know that the increased time comes with the extra accuracy of the finished parts. Are there any other methods for this type of project that you could recommend for improving efficiency and not sacrificing? Could I somehow convince my wife that a VFD spindle would make me work faster? Perhaps the answer is to make all of my large rectangular cuts off the machine, and bring to the machine for the rest of the detailed work.

I had a few small follow-up questions related to some things you mentioned. I went through the learning content on https://my.carbide3d.com/ a year ago when I first got the SO 5 Pro, and that amount of learning has gotten me by for basic projects like the simple signs I’ve made, but I’m realizing there is still a lot to learn.

Regarding the cutting depth being almost 3 times the diameter of the tool - Is this problematic in general?I assume maybe you mention it because the depth of the stock is a contributing factor for the slotting effect being more dramatic, and if I was doing the same cut on something much thinner the effect may not be as drastic? Would love to know more about this and if there are general rules of thumb to follow as it relates to the ratio of cutting tool diameter to stock thickness or total depth of cut.

Regarding the “working inside out” method - What importance does this have to arrange the cuts in this manner? I assume that this method would reduce the risk of an “inside” cut breaking a tab and causing something you’d previously cut on “the outside” to fail. Are there other reasonings for arranging the cuts in this manner?

Finally, is there a good comprehensive resource (wiki, book, course) on CNC Best Practices or Principles that would answer a lot of these types of questions? I know in my 3D printing hobby, most of my knowledge has come from trial and error over the last 8-9 years. However, mistakes on the 3D printer are much less costly.

Thank you again for all of your help, Will. Have a great rest of your day!

[WillAdams (William Adams (Carbide 3D))]

See:

Introduction

and for more software-specific things:

2D Drawing

and

Toolpaths

The big thing to remember is that the machine has no sensors while operating, save for when homing, so one has to keep feeds, speeds, depth per pass, and tooling engagement low enough that for a given number of revolutions of the cutting tool and matching steps by the stepper motors there is a certainty that the torque of the motors will be able to accomplish said steps.

[rob5standingby (Rob)]

These are awesome. I had not seen these two Gitbook pages. Thank you so much for everything, Will!

[gdon_2003 (Guy Donham)]

@WillAdams advise is good and you should follow it. However if you are still not exact then there are many posts about calibration here on the forum. On the SO3/4 you are compensating for belt stretch. On the SO5 there are no belts but you can change the gbrl parameters to get your steps adjusted so you are right on. If you customize your steps every time you run the configuration you will need to either re calibrate or write down the numbers you create to calibrate and reenter them after a configuration.

Before calibration make sure everything is mechanically correct and you have lubricated your rails and bearings.

[pcperks (Phil Perks)]

Also check the bits you use, because if you are getting Amazon specials they may not be the exact size that they say they are. Over large areas, that small difference can add up.

[abcnevin (Andrew Nevin)]

Whenever I see a pattern (1/16th under) on all sides, I go back to the basics: Which tool did I have actually loaded (diameter issues vs software etc), does the “right outside” toolpath actually create the desired contour path with the correct radius offset, little things like that can save you a lot of time vs square/level/tram/recalibrate/etc your machine. I don’t doubt your abilities at all, we have all made beautiful kindling at some point!

[rob5standingby (Rob)]

That is a great reminder, and definitely one of the first things I went to check! Did I use the right tool, did I set the offset on the contour properly?

[rob5standingby (Rob)]

Great point! Just using the #201 bits from Carbide at the moment, but it wouldn’t hurt to verify their dimensions.

[rob5standingby (Rob)]

Thanks, Guy! I am going to try out Will’s recommended methods with the cutting pattern changes (pocketing and avoiding slotting), but also definitely going to look into whether or not the steps are calibrated properly. I found a link on the methodology for the step calibration in the Gitbook that Will linked: Dimensional accuracy - Shapeoko CNC A to Z. I have certainly experienced a very similar thing with stepper calibration on my 3d printers over the years.

[SLCJedi (Josh Tenny)]

1/16" of an inch is way too much to be a calibration issue. If you were 0.020" or less, I would say calibration. But the equal all the way around, consistency, and common dimension lead me to believe it is most likely in the programming or set-up.

I would also agree to check endmill diameter, and the actual designed size. I have accidentally sized something incorrectly more times than I would like to count.

[rob5standingby (Rob)]

Thanks Josh! Are you suggesting that possibly the Carbide branded #201endmill paired with the Carbide Compact router is not a good combination to cut a cabinet panel from 3/4" baltic birch plywood?

As far as set-up and programming go, I still haven’t had time to get out into the garage to try Will’s advise for pocketing the large area before making the final pass. I saw a video a while back on Carbide’s YouTube channel where Kevin made cabinet panels, and I don’t think he did anything too crazy in terms of how he cut them out, it appeared that he just did the ‘slotting’ technique that is recommended to be avoided.

[SLCJedi (Josh Tenny)]

@rob5standingby

Are you suggesting that possibly the Carbide branded #201endmill paired with the Carbide Compact router is not a good combination to cut a cabinet panel from 3/4" baltic birch plywood?

That combo should be good. I’ve never known one of C3D’s endmills to be off more than 0.001" from nominal. The router has more run-out and less concentricity than their spindle, but also, shouldn’t come anywhere near 1/16"

I’ve cut a lot of slotting profile cuts and never seen more than 0.020" from nominal unless I had a mechanical issue or I made a design/programming mistake. And I have owned or ran 7 different Shapeokos. That 0.020" was on my first Shapeoko 3 before I did calibration for things like belt stretch. I’ve just never seen that high level of variance out of a belt driven Shapeoko, let alone my S5Pro. I think my 12" test square and circle (both cut as a slot) were under 0.005" from nominal on my first test cuts with my S5Pro.

Background: I was a machine operator in aerospace for almost a decade. I also machine almost daily at work…often on our Shapeoko 4Pro XXL or HDM. Both of which make scientific level parts for experiments.

[Rizzo (Eric Risbrudt)]

Wow, so much information to take in and digest. Great stuff here. I haven’t tried to be 100% accurate on my designs yet as it was not critical. However, I was just thinking about making a Y reference with some maple as I saw from C3D online, and wanted to see how accurate I could get the S5P. This gives me something to go from rather than get to. I’ve spent about 30 years as a Tile contractor (now done with that) and am learning this trade. There is so much that it is mind blowing. I’m having a great time learning and doing; its humbling when you’ve started thinking that you’re getting it all and then a little info nugget like this pops up. Thanks all!!

[downrazor11 (Stephen)]

Is the top-across the same as the bottom-across? Deflection may play a part as well…

[rob5standingby (Rob)]

So I have gone down a rabbit hole!

I have yet to work up the courage to try cutting another piece of expensive Baltic birch but I decided to eliminate a few other possibilities this evening.

I had verified a handful of times that my program dimensions weren’t wonky, and that I was measuring the width from the top edge as well as the bottom edge that was facing the spoil board.

I verified that my carbide #201 bit was indeed the right diameter, so that is good!

I then decided that a reasonable thing to do would be to eliminate the cutting from the equation and first verify that the stepper movements were accurate, despite everyone telling me that these should be calibrated from the factory. I’m hard headed sometimes, I suppose.

I decided to try and build a rigid sharpie mount which had no play in the X and Y directions, but allowed for movement in the Z direction. This was probably a very unnecessary rabbit hole to go down, but I had fun. I found some old 3D printer parts in my parts bin and designed the monstrosity you see below. It’s quite stable in the X/Y direction but will allow the pen to move upwards in the Z direction as the Z axis is pressed into the work piece. There are two linear 8mm bearings which keep the movement smooth and almost entirely isolated to the Z axis. I am aware there are simpler ways, but I had fun making this.

I then programmed a simple set of rectangles of various sizes on my 2’ by 4’ bed, and I traced them out on a sheet of MDF, and measured the rectangle sizes. I know this isn’t the most scientific method, but I thought my results would be decent given that the sharpie isn’t able to flex in the X/Y.

Anyway, my rectangles were drawn quite nicely by my crazy attachment contraption, and they all came out measuring exactly the dimensions I’d entered in my design file in Carbide Motion! So I am now confident that I can eliminate stepper calibration from the list of possible issues.

I suppose I now have a little sharpie attachment which I think I’ll try to use for some drawings. The pen holder can be removed with a thumbscrew so you could theoretically hot swap a few different colors and leave the main assembly attached.

I will be moving back to trying out some actual cuts now and attempting a few of the methods recommended by Will. I went down a very unnecessary rabbit hole for a few days working on this sharpie mount, but I had a lot of fun.

[gdon_2003 (Guy Donham)]

I have read this post on and off. You got a lot of advise that is good. One thing I am not sure was covered is when doing a contour you can give no offset, inside or outside. Did you possible pick inside which would result in a smaller dimension than you intended.