X50 Hole Diameter is inconsistent in my Wasteboard

1

I’m using Fusion 360 to cut my wasteboard.

I designed it to have a bunch of dog holes in them.

I just came out to see how the machine was doing and all the holes are cut, but the bench dogs either slide in really nicely, fit snug, or don’t fit.

It seems like as the machine moves to the right (x axis) in general, the holes get tighter and tighter. It’s not everyhole, but almost all of them on the right side don’t fit, where as all of them on the left slab fit.

Autodesk_Fusion_360
Autodesk_Fusion_3601920×1320 156 KB

As you can see in the picture, there are lots of holes, but from the middle slab on over, most of the holes are to tight.

I did surface the board, and when I looked at it, inspecting for tramming issues, while I could see some lines in the boards, to the touch they were pretty hard to feel so I don’t think it’s a tramming issue.

The holes on the left slab are cut to about 19.87mm but the holes more on the far right slab can be as small as 19.73mm.

But also I can say that on the far left slab holes can range from 19.87 to 20mm.

So the machine is always off, but just more off as the slabs on the right of the machine are cut.

What would cause this?

Here is a picture of it installed.

ACAD17F8-ACF8-4FC9-A720-1422E195F766
ACAD17F8-ACF8-4FC9-A720-1422E195F7664032×3024 3.17 MB

2

In addition to the calibration tests I suggested in the other thread it is possible the runout of the router is increasing or decreasing as it heats up and tool wear/dulling of the cutter leading to more deflection could be a factor if they became tighter later in the milling operation.

1 Like
3

Interesting, so i just ran the hole pattern again on the far right slab only. And as it has done 5 or six holes, the bench dogs now fit nicely in the holes.

What would that make you think?

4

Hey Mark, hey Derek @WaywardWoodworker,

First I was thinking of the same possible cause as Derek, that you have a sharp bit first and on the right it is increasingly dull. But what you are reporting now speaks against it.

The next question could be, how do you multipicate the holes in your 3D model to create the final model? By copying groups of holes?

When you say, you just milled on the far right slab only. Did you use the part of the model that was used on the left first, or the part that was made for the right? I assume you have a model for the entire wasteboard.

5

Good question. I just selected the holes for the far right slab. See attached screenshot.

QTView__3_Browser__1__and_Autodesk_Fusion_360
QTView__3_Browser__1__and_Autodesk_Fusion_3601920×994 128 KB

1 Like
6

Hey Mark,

interesting. That could mean the diameter of the holes change with increasing heat of the bit. The cutting edge of the bit might behave differently. You said the diameter of the dog holes decreases from left to right.

What kind of bit is it? When milling wood, the heat is evacuated by the chips, so good chip evacuation keeps bit and wood cooler. That’s why high spindle speeds are important on wood milling.

1 Like
7

This is the bit:

Yea, the machine did cuts from slab 1 ( far left) to slab 5 (far right)

And while in general the holes are smaller as we move from slab 1 to slab 5 there are incosistencies in each slab (even in slabs 1-3) i can take the same bench dog and slide it into some holes and its really snug and then try another hole just a few away it its a little loose.

I’m using the makita cnc

The speed is set between 2 & 3.

Which based of this picture:

image
image368×691 27.1 KB

is somehwere close to 16000 rpm.

I’m new to all of this btw so I don’t really know if i’m using the right bit, the right speed, … so all thoughts and wisdom welcome.

8

My vote is but deflection. That is a long bit for typical waste board thicknesses. What’s your cut depth?

In VCarve I’d be doing a spiral cut and using a shorter depth of cut bit - like 1" max.

1 Like
9

Well the thickness of the mdf was originally 3/4”

But I did shave a bit off when it was surfaced.

Am I using the wrong kind of bit aside from it being a little longer.

I had chosen it initially so I could cut the threaded inserts that screw into the actual bench top. ( which allowed me me to have screws that hold the waste board down)

10

Here is another interesting thing. So on this second pass as i just to slab by slab, the hole are almost too loose.

But what is more interesting, is that the bench dog moves more side to side (along the x) but if i try to wiggle the dog forward and back(along the y) it doesn’t move that much…

See video.

This is a bummer because now i feel like i’m going to need to remake these slabs… thats a 1mm or so of play from left to right.

So i guess the first thing i’ll do is use use a ruler and see if the machine is correctly moving from left to right.

Then maybe a different bit?

11

Hey Mark, hey Jim,

I agree with Jim that while this bit may be good for the long holes for the threaded inserts, for dog holes where fit is important, I would apply the general rule not to use bits longer than absolutely needed. Deflection is an issue easily. Can you repeat the dog holes with a shorter bit and see if the problem gets better?

By the way, if you use the Makita hand router, which is a so-called universal motor, you should know that this is a type of motor that is slowed down by applying mechanical load. The electronics try to prevent that, but the fact that you have no torque at high speed on this type of motor cannot be circumvented by the electronics (for difference between universal and induction motors regarding torque and speed, see here). So on a hand router, the speed setting is usually only the speed with no load. Spindles on VFDs hold the speed independently of the mechanical load (up to the current limit set in the VFD, then they abort with error and, if safety wiring is correct, they interrupt the CNC program. See here for spindle just before the limit :slight_smile:)

1 Like
12

Hey Mark,

That’s the next thing I wanted to ask, are the dog holes smaller in all directions, or oval in X direction.

By the way, on my browser, your video says:

What codec is it? I hear only the audio :frowning:

I would make a program that makes marks with the tip of a v-bit at specific distances and check the distances after you ran the program.

Absolutely, with length only as needed, since deflection is easily an issue. Two-flute upcut with a medium angle spiral is okay. You could use a larger diameter for dog holes.

2 Likes
13

Ok. I re-encoded it with h264 the default was aac which i guess the browser didn’t like.

Yes. Now they are now more oval (along the x axis) from 19mm to 20mm. (DOH!!!)

The Y still seems pretty good… but the x is messed up now.

1 Like
14

Hey Mark,

thank you, I can see the video now.

Wow, what a play in X direction.

15

If the x & y diamters of the holes are different. Is that clueing us in to it being a bit length / deflection issue or more of a calibration issue?

16

I would first try out to make the same dog holes with a shorter bit. I assume you have some material you can use for tests.

For checking the machine accuracy, as said above, I would first make make a program that makes marks with the tip of a v-bit at specific distances and measure the distances after you ran the program. This would be the no-load test. Next step would be to mill holes or pockets with a higher feed rate to have higher load and measure the results then. I would measure the diameter of holes or the width of pockets with a caliper, as well as measure the distance between holes/pockets that are far away from each other. This way you could see where accuracy is good or not.

1 Like
17

Yea. i have a few more little pieces of MDF

And i have the shorter version of that bit:

*Astra Coated* 1/4" Up-Cut Spiral Router Bit - BitsBits.com.
( side question: What bit would you think would be ideal for making dog holes?)

I’l update to use the shorter bit and test the hole really quick.

Then i need to figure out how to do this mark test.

Would you use a vbit for that?

I have 2.

This one:

And this one:

I’m not really sure how to pick which bits to use yet.

Also i have this caliper that my dad gave me…

2963B165-B335-4430-AA95-F4228B908273
2963B165-B335-4430-AA95-F4228B9082733024×4032 2.52 MB

18

When do your calibration testing make sure to design your program to test backlash. Don’t only increment in the positive direction. Test positive, negative, and a combination.

1 Like
19

Could you elaborate a bit more?

This is all new to me.

1 Like
20

@Aiph5u I just redid a hole with the long bit, then switched the bit to the shorter bit, updated the gcode (updating the tool to the new bit of course), then ran the same hole and the long bit has play, the short bit doesn’t.

So i’m thinking that confirms it has something to do with the bit and not the calibration of the machine.