AR16 cutting square issue

[nergles]

I just assumed out of the box the AR16 is squared and trammed but im beating my head against the wall as a newbie to CNC in general and just want to try and figure out what im doing wrong. 


Hello everyone! I am going to cross post this to a few different groups I’m in and I apologize if this is not permitted and or see you it due to that overlap. I am having an issue with my new Axiom AR16 and I can’t seem to resolve it and unsure if it’s user or machine error.



I am having issues with the same 2 corners on every cut I do. I have tried different files, redrawing my art, I leveled the machine again today, lowered the speeds, and tried different bits its always the same thing regardless of what I’m cutting its the same thing.



Axiom AR16



Amana Bit Spektra bist Axiom sell



Checked Aspire for node issues



Seeing lots of chatter and or material on floor. Does it need to be trammed?

Images of the issues were uploaded here:

imgur.com/a/L7pe1Zf

[gerry]

Sept 15, 2019 20:32:22 GMT -5 nergles said:

Seeing lots of chatter and or material on floor. Does it need to be trammed?

Looks like you're over-driving the machine, losing steps.

[johnb]

From what I see from the chewed up surface of the pocket cut and the consistency of the "errors" in the letter shapes (the same "glitch" extends the whole depth of the letter), I would surmise the following:
1) You seem to be cutting the whole depth in one pass. Decrease your pass depth.
2) Your spindle speed is too low and your feed rate is too high.

Did you draw this yourself or use a letter font? The whole thing looks pretty ragged. If you drew it yourself, go back to Aspire and expand the size of your image to see if it looks as good as you think it does.
Also, you would probably be well served to download Version 10 of Aspire (just out). One of the new features is a chip load calculator. Check around and see what kind of chip load you should be seeking for a given bit with the grade of MDF that you're using.

What Gerry said about overdriving...The AR-16 Elite uses servo motors, not stepper motors. The difference in the two is that a stepper motor "assumes" that the spindle went where you told it to go. Lost steps tend to result in dramatic garbage for the rest of the file run because the spindle isn't where the controller thinks it is. With a servo, you can still "get in the wrong place" in the material when you bog down the bit, but it's constantly communicating with the controller and it will "get back on course" to where it is supposed to be. I haven't ever had anything come out looking like this, but I suspect that too much feed speed and too much depth would result in just this. The reason I think your spindle speed is too low is that the bottom of the cut (and some of the edges) are shredded. That would result from the bit being moved past a given point in the material before the bit makes enough revolutions to clean up the cut.

The chatter you describe and stuff "flung to the floor" would tend to bear all this out. You want chips...not chunks (or sawdust).

You might want to consider a finish pass with an offset as well.

[Mezalick]

My suggestion is to step back and start from the beginning.
Look at the software parameters you're using.
As said by others, feed and speeds, and cut depth.
It looks rather agressive of a cutitng approach.
If you want to send me the file I can take a look at it.
Michael
[e-mail]

[nergles]

Thanks for the feedback guys. Regardless of the file, this happens on the same exact 2 corners period. on the first picture, it was .150 depths on a .25 endmill. at 100IPM. I find it hard to believe that is considered aggressive for the machine.

In the MDF here it was 100 IPM and open a 1/8 end-mill it was 3 passes but ill need to verify tomorrow the depths. 

[johnb]

Other considerations...(I'm not trying to insult you here, but)... let's "begin at the beginning", and ...by all means, at least send Michael your file (even if you don't want to post it here).

1) Did you seat the collet in the nut completely...with an audible "click"...before inserting the bit?
2) Is your work piece adequately restrained on the spoilboard?
3) Is your MDF bowed and not sitting flat on the spoilboard?

The uneven pocket and triangular "islands" (and the ridge at the base of the letter at the top of the 4th picture) would indicate that one of the above problems exists.

If the work piece is bowed, then that "changes" as more material is removed and the tension of the bow is "relaxed", resulting in the bottom of the pocket being at a different "altitude" during further passes.

The tendency of the bit to want to "lift" the workpiece can also produce this. This may not be readily apparent to you. If you're using only the linear and straight-sided clamps to hold your work in place, then you aren't providing adequate grip on the work to prevent it from being lifted off the table. This is not a particular problem when V-Carving, because the geometry of the bit tends to not have a "lifting component" in those cuts, but a straight end mill is providing upward thrust that increases as the cut deepens and more of the "wall" of the cut is in contact with the bit.

Not challenging what you said here, but those pocket cuts in the MDF sure don't look like they were made with a 1/8" end mill to me.

As far as those ragged edges are concerned, unless it's "baked into" the vectoring in your file, either the bit is not in the collet securely (see #1) or the work is being moved around on the table during the toolpath.

4) Are you ramping into your cuts?
5) What is your Z plunge rate?

[Nergles2]

No insult this is my first dive into the CNC world for all intensive purposes and I'm 100% open to it being user error.

I have no issues sharing the file my only hesitation is it says harley Davidson as I was using it as my test cut. I dont want to get in trouble for that. The out profile cut was down a .25 end mill.


I I've done multiple bit changes and recieved the same situation gosh I guess it's possible I've been putting it in wrong these times just seems unlikely. I'll reseat everything again and perform a test cut.

I looked very hard and saw no movement of the work piece. We fixtured it pretty snugly there.

Thank you guys for the responses and again no offense I'm stupid when it comes to these things and I'm not ignorant to that.

[Axiom Tool Group]

We'd be happy to take a look at the files as well.

What post processor are you using?

[nergles]

Here is the most recent version and I will upload new pictures where this is 1/8" bit at 50IPM on MDF and same results.

File Download: gofile.io/?c=hRZva7

New Images :https://imgur.com/a/1vJfklK

[Mezalick]

Sept 17, 2019 11:44:41 GMT -5 nergles said:

Here is the most recent version and I will upload new pictures where this is 1/8" bit at 50IPM on MDF and same results.

File Download: gofile.io/?c=zIubks

New Images :https://imgur.com/a/1vJfklK

I get an error message when I try to open your flle.

It appears that you are using Aspire 9.51.

Do you own the software or is this someone else's file ?



Thanks

Michael

[Axiom Tool Group]

I'm getting errors as well...I can't open it with 9.518 either.

[johnb]

It would not open in Aspire 10.0 either. I did research the error code (126663) and found this post regarding that on the Vectric Forum:

"Whenever I get a file that generates an error, it is invariably from a student who jerked out the thumb drive before the software was done with it, or closed/crashed the program before it was done saving the file. The file is corrupt. When I've received a file from a trial version the software states that as the reason it won't open it."

[Mezalick]

Can you resave the file as a Version 10 and send it to [e-mail]...One issue with the error message is that you may not be giving the computer enough time to save the file..In my hetic work schedule I ofter do this,,Thanks

[johnb]

Another question. You mentioned tramming the spindle. I assume that you haven't done that, but did you surface your spoilboard surface before you began your first project?
If that was done, then the spoilboard is (for sure) coplanar with the gantry/spindle travel. If you ended up with a nice smooth surface from the (wide diameter) flycutting bit, then your spindle is NOT out of tram. If it were, you'd have ridges in the direction of the raster of the spoilboard smoothing file.

When I flattened my spoilboard, after zeroing the Z at the midpoint of the X travel, there was definitely more removed from the Minimum X side of the spoilboard than there was from the Maximum X side.

I've run out of ideas as to why the bottom of your pocket cut is so ragged...other than the fact that the stepover appears to be nearly 100% of the bit diameter in (at least) your final path on the bottom of the pocket.  

[nergles]

Thanks for the feedback please find the correct file located below.

gofile.io/?c=hRZva7

In addition, I did speak to Craig today who had mentioned doing a spoilboard pass and I can confirm I have not done this yet. We just received the machine in 2 weeks ago or so and are just now getting to setup and usage.

[johnb]

AFTER you've flattened your spoilboard, do this

I think the problem is in the Harley Davidson-7.ai file that you imported. If you change NOTHING in the file and preview the toolpaths, that comes out looking pretty crappy.

Start over and use the text tool with an appropriate font and continue from there. Also know that, unless you're cranking it down with the dial on the HUST controller, you've set the spindle speed to 18,000 rpm. That's a 2 flute bit and you would need to drop your spindle speed to 12,000* and up your feed rate to 100 ipm to come up with a chip load within the optimal randge (for MDF) of .004" to .007"

This file also shows that your are using a 1/8" end mill with one single pass of 1/8" for a cut depth of 1/8". You may be getting bit flex as well. It takes longer to make 2 passes (but remember, you're upping your feed rate), but try going 1/2 that depth and making 2 passes.

* Note that...on this machine, the spindle speed is NOT set by the software, it's only set on the controller.  The maximum feed rate can be set in the software, and decreased at the controller (but cannot be increased beyond the feed rate that comes over from the software).

[nergles]

Do you have any guides or youtube recommendations for creating the file for the spoil board?

[Gary Campbell]

Try this to start:

[johnb]

Sept 19, 2019 14:13:13 GMT -5 nergles said:

Do you have any guides or youtube recommendations for creating the file for the spoil board?

It came with the machine. Look on the flash drive that they sent (Mine was in the (obviously opened) original packaging for the drive.)

If it doesn't smooth the entire surface of the spoil boards, I can tell you how to fix that too.