Welcome to Our Community

Some features disabled for guests. Register Today.

Workbee accuracy - adjustment - calibration

Discussion in 'CNC Mills/Routers' started by Felix_Hauser, Dec 7, 2019.

  1. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    Hi all,

    First time posting here, I hope I haven't overseen anything. I will cut to the chase.
    I own a 1000x1000 Workbee, screw driven and with a Duet as a controller board and the latest firmware (as of December 2019). Yesterday I was working on a small box I designed in Fusion 360 (for which I have the corresponding post processor). I wanted to create a couple for inserts for a very small brass hinges and when it was done with it, I realized that the measurements were a way off, compared to the values on Fusion. I am well aware that the measurements never translate one-to-one on these hobbyist machines, but I am talking of an error of 0,70mm over a value of 20.00mm. Taking into account that the reported accuracy of the machine is from 0,05 to 0,1mm, I think 0,70 is way off... I proceeded to check the steps/mm of the motors and to my surprise I notice that the motors were not moving the same depending on the direction. For example on the X axis, with the same requested distance, the actual distance was not the same if moving to the right or moving to the left. That led me to think that I had either a problem with the motor couplers or with the backlash nuts, or with both. So today I spent some time to adjust everything a little bit: the tension of the wheels (which I left to the "default"), the couplers (which I left with the motor shaft in contact with the drive screw), I loosen the backlash nuts and tightened them again and I put some grease on the screws. After that I squared the Y axis, I rechecked the movement and, to my enjoyment, the distance was equal no matter the direction. At this point I calibrated the steps/mm and started the box from scratch again. When I finished on of the parts, I measured it and contrasted the values with the expected ones. The result are as follows (see attached picture for clarification):

    d1: act.= 72,70; exp. 72.00
    d2: act.= 40,65; exp. 40.00

    d3: act.= 60,08; exp.= 60,00
    d4: act.= 24,94; exp.= 25,00

    So, what I can see is that compared with the first box, the measure of interior dimensions (d3 and d4) are way more accurate and well within what I expected. The exterior dimensions, however are consistently aprox 0,70 larger than the ones in fusion. The box will be perfectly usable, but I do wonder about why some dimensions are pretty accurate and the other are consistently larger. More info: external dimensions are a contour operation in Fusion whereas internal dimensions are from a 3d adapting clearing operation (without "stock to leave" and/or contour operation as finishing). The dimensions of the endmill are accurate.

    Any insight in understanding this will be much appreciated. Thanks in advance!
     

    Attached Files:

  2. jeffmorris

    jeffmorris Well-Known
    Builder

    Joined:
    Nov 6, 2017
    Messages:
    315
    Likes Received:
    56
    Did you measure your bits? Some bits are not exactly the size listed on the pack. For example, a 1/4" bit is really 0.24" instead of 0.25".
     
    Giarc likes this.
  3. phil from seattle

    phil from seattle Well-Known
    Builder

    Joined:
    Mar 17, 2017
    Messages:
    181
    Likes Received:
    83
    Look at your G Code to see what it's trying to do. It'll take a little work to figure out if the GCode is the culprit. a spreadsheet might help. Given that your interior measurements are basically correct, it doesn't make sense that the machine is off. My first thought was the infamous "stock to leave" error that catches a lot of people but I think you said it wasn't the case (I'd double check anyway).
     
  4. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    I did, in fact, measure the tool and instead of 3,175mm of diameter (1/8") it is 3,13mm. That makes it for (3,175-3,13)*2= 0,09mm of error (about 3 tho), but not for 0,7mm. Good point though, I forgot to mention it.

    After I posted my question, I did some extra research and I came across a thread on the Fusion360 forums. To summ it up, a gentleman was experience similar problems and after much discussion, it was found out that he had the "Cutter Compensation" setting set to "mill climbing", which apparently can cause some problems with hobbyist machines such as mine. I did check my settings on the contour operation of my CAM and, it was also set to "mill climbing". This is one of these settings which is set by default and it is hardly ever discussed. Because I am a noob, I did not even looked at it.
    Today I have some work stuff to do, but when I'm done I will try the contour again by changing that setting to "conventional" and I will report back here. I am very curious about it.
     

    Attached Files:

  5. Alex Chambers

    Alex Chambers Master
    Moderator Builder

    Joined:
    Nov 1, 2018
    Messages:
    1,191
    Likes Received:
    558
    Hi @Felix_Hauser, you should only ever use a DRY lubricant (silicone or ptfe) on your leadscrews - oil based ones can attack your nut blocks and trap (abrasive) dust.
    On the accuracy issue try setting a roughing toolpath (leave say 0.5mm of stock) and then do a final cut (full depth) to take off the last 0.5mm.
    Alex.
     
    Felix_Hauser likes this.
  6. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    Thanks for the tip!. I used general purpose grease. Good news are, I only did a small job after that. I will clean them off and put some silicone oil.
     
    Alex Chambers likes this.
  7. Alex Chambers

    Alex Chambers Master
    Moderator Builder

    Joined:
    Nov 1, 2018
    Messages:
    1,191
    Likes Received:
    558
    Use a DRY spray - nothing liquid.
    Alex. :thumbsup:
     
    sharmstr likes this.
  8. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    As I promised I have just done another test, right now. I did a 3d adaptive clearing operation just like the one before and also a 2d contour operation with the Cutter Compensation setting turned to "Conventional". All of this, after I replaced the grease on the lead screws by silicon oil.

    The results are as follows:

    External Dimensions (2D Slot operation):
    d1: act.= 60,25; exp. 60,00
    d2: act.= 40,42; exp. 40,00

    Internal Dimensions (3D adaptive clearing operation)
    d3: act.= 39,81; exp.= 40,00
    d4: act.= 19,62; exp.= 20,00

    So apparently the whole situation has worsened. The good news is that the Z dimensions are only 0,01mm short of the expected value, so I have this going on for me.
    I also must say that I did the test on a scrap piece of Plywood. I do not want to waste nice oak just for doing tests like these, but I know I introduce another variable into the equation here.

    Again, I do not expect a Haas precision here, but if I could have a more precise comfort zone, it would be great. I think a 0,38 or eventually a 0,42mm can be improved even in hobbyist machines.

    Any further inputs are welcome...
     
  9. Giarc

    Giarc Master
    Moderator Builder

    Joined:
    Jan 24, 2015
    Messages:
    1,382
    Likes Received:
    725
    It has been a while since I used Fusion to generate gcode. Is there a way to not select any compensation? I do not recall ever using any compensation and I have not had parts cut that far out of spec. I cut a 25 mm hole last night and a 25 mm part to fit in it and it was a perfect press fit, so it is doable with these machines. I used Estlcam to generate the gcode and there is no selection for any kind of compensation to which I am aware.

    Also, you mentioned you measured your endmill and said you expected the cut to be off by about 0.09 mm. However, you never confirmed you entered in that dimension into Fusion - unless I misread. I assume you did, but I just wanted to be sure.
     
  10. sharmstr

    sharmstr Master
    Moderator Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,057
    Likes Received:
    645
    Hi Felix,

    "Cutter Compensation" is not the correct terminology. We know what you mean, but others wont since it has nothing to do with either climb or conventional milling. (Cutter Compensation for Beginners - Fusion 360 Blog) (EDIT - See giarc's comment above. he thought you were really talking about cutter comp when you're not)

    Can you clarify the actual operations you are running? If I understand, you are running a 3D Apdative on the pocket and a 2D contour around the outside of the box you are making. If that's the case, then you need to add two additional operations.

    For the pocket: 3D adaptive is a roughing toolpath and Fusion will default to a .5mm "stock to leave" value because it assumes you'll apply a finishing toolpath next. If dimensions are important, you will always want to follow this toolpath with a finishing toolpath. So, go into your 3d adaptive, click on the Passes tab and verify that you have stock to leave set. If you do, that's why its undersized. But like I said, you want this. Add a finishing toolpath all full depth with 0 stock to leave to clean that up. You can also uses that finishing toolpath to dial in your dimensions but adjusting the stock to leave. (get used to doing that for critical dimensions)

    Same theory applies to the outside contour. Cut it using multiple depths with some radial stock to leave. Then add a new toolpath a full depth and dial in the fit.
     
    #10 sharmstr, Dec 8, 2019
    Last edited: Dec 8, 2019
    Giarc likes this.
  11. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    Thanks for all the info and insights Giarc and Sharmstr. I used the term Cutter Compensation because it was named like that in the post I saw. I posted a screenshot of it a few posts above.
    Today I had to work (or rather prepare for next week) and I did not have that much time. On a pause I did this afternoon I re-calibrated the steps/mm of both X and Y since last time I did that I was moving only 10mm. Today I did it with 100 instead. I made 10 reading per axis, 5 in each direction and I disregarded the highest and the lowest values. With the 3 remaining values I calculated the average. The values of each direction were consistent, so no problems there.

    A few minutes ago, I run another test using the measurements of the hinge insert I want to do. I created 3 pockets on Fusion with different sizes. You can check the results on the attached image. If we eyeball it, one could see an average -0,20 mm error.

    This is how I did the manufacturing:

    • 3D adaptive cleaning with stock to leave radial set to 0,5
    • 2D contour with conventional sideway compensation as a finishing toolpath
    • all of this with a 1,5mm Endmill

    I'm trying to find the file to attach it, but I can't find it. Maybe it hasn't been saved the cloud.

    Anyway, somehow I'm getting closer. Now it's more consistent...

    EDIT: I found the file, here is the public link. I hope it works

    Fusion
     

    Attached Files:

    #11 Felix_Hauser, Dec 8, 2019
    Last edited: Dec 8, 2019
  12. sharmstr

    sharmstr Master
    Moderator Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,057
    Likes Received:
    645
    As I mentioned before. If you want dead on accuracy, you're going to have to dial in your toolpath using stock to leave. Even the HAAS kids have to do it. That .20mm average didnt take into consideration your undersized endmill, right? .11mm aint bad for a hobby machine.
     
  13. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    I think you‘re absolutely right. The CAM side of Fusion is still a very uncharted territory for me. However, as I mentioned, in my last test I did leave „Stock to Leave“ turned on to the default 0,5mm and I did a final 2D Contour pass as a finishing pass. It is the right way to do it? I don‘t know, to be honest. The other thing is that for these tests I used a 1,5mm endmill. Today before I left for work I checked and it is quite dead on 1,50mm.
     
  14. Wallied

    Wallied New
    Builder

    Joined:
    Sep 9, 2018
    Messages:
    25
    Likes Received:
    11
    Yes, you're quite correct in the roughing - finishing department. But one thing to note is the fact you used a very fragile bit, which is prone to deflect, which in turn reduces your accuracy. There are many opinions on the finishing stepover (stock left by the roughing operation or passes), Personally I try to go between 0.2mm and 0.8mm on wood, depending on the bit diameter. In this case I'd go with 20% of the bit, so 0.3mm. Ideally you would use the largest bit that allows you to make the cut for the best accuracy and finish quality.

    But realistically I'm inclined to believe that all the remaining inaccuracies in your machine are due to backlash, the physical limitations of the machine, spindle runout or something along those lines, and not anything with your CAM. And if I remember correctly, Ooznest promises 0.2mm accuracy for the Workbee, so you're right about there, and there's not much more to be done.

    However, since your travel distances apparently are too short all through the line (in both directions, and both on the inside of pockets and outside contours), you could play with the steps/mm setting some more to see if you can close in on the nominal dimensions.
     
    sharmstr likes this.
  15. sharmstr

    sharmstr Master
    Moderator Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,057
    Likes Received:
    645
    I totally forgot about runout. That's a big one.
     
  16. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1

    Ooznest claims an accuracy between 0,05 and 0,10mm, which I must say, it's hard to believe. It sound a lot like the car commercials where the efficiency is measured in a closed circuit on a dry, wind-free day and at a constant and controlled speed...

    Is there any way to measure backlash? or check out if there is any? What is spindle runout, btw?
    I don't know if it accounts for anything at all, but I ordered some other motor couplers, the ones delivered with the machine do not seem adequate for the ammount of stress. I got some of those with a cross shaped rubber piece in the middle (I don't know the correct denomination)
     
  17. sharmstr

    sharmstr Master
    Moderator Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,057
    Likes Received:
    645
    Both are easy to check with a dial indicator. Here's a few videos on the subject




     
  18. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    well, that goes the one NYC CNC video I haven't watched yet... thanks!
     
  19. sharmstr

    sharmstr Master
    Moderator Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,057
    Likes Received:
    645
    No prob. John has some good vids. Its why I went with Fusion and why I bought a Tormach.
     
  20. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    9
    Likes Received:
    1
    Well, I ordered a Mitutoyo dial indicator (2110s-10) and I calculated the backlash on both X and X axii.

    X: 0.0010 mm
    Y: 0.0015 mm (the hand was between 1 and 2)

    I´m guessing is not that much of a backlash error, I assume
     
    #20 Felix_Hauser, Dec 15, 2019
    Last edited: Dec 15, 2019
  21. Alex Chambers

    Alex Chambers Master
    Moderator Builder

    Joined:
    Nov 1, 2018
    Messages:
    1,191
    Likes Received:
    558
    The accuracy of your workbee will depend on how well you put it together, but on my drivescrew 1010 I achieve better than 0.1 mm. In the real world you also need to take into account the actual tool size, tool runout and tool deflection.
    Your backlash readings are excellent, but check them from time to time - things sometimes work loose and backlash nuts wear.
    Alex.
     

Share This Page

  1. This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
    By continuing to use this site, you are consenting to our use of cookies.
    Dismiss Notice