First multi-hour carve. Asking for some analysis

X-Carve
1

I finally did a multi-hr carve with my new 1000m. Overall the carve took about 3 hours with a roughing and finishing pass. I was very happy with the results for my first more complicated carve. There were a few items that made me wonder.

35
351280Ă—895 626 KB

The parms I used are:

Rough: .25" 2 flute bit, 60 ipm, 30 ipm plunge, .1 doc, 40% step over. Dewalt at 2.
Finish: .0625" 2 flute bit, 60 ipm, 30 ipm plunge, .003 doc, 40% step over. Dewalt at 2.

The wood is poplar.

First off, during the roughing pass, I had some slight chatter occuring during long, straight cuts on the X axis. I tried speeding up the feed rate, slowing down the feed rate, speeding up the spindle, slowing down the spindle, combination of previous, etc… I ended up back at 60" at setting 2. The only thing I did not try to reducing the DOC.

I’ve attached a video trying to show the chatter.

Is this normal, minimal or extreme amount of chatter? What can I do to reduce or eliminate?

In the second picture, there is a line that happened across the “S” indicated by 1. Also there was some roughness left indicated by 2. Any ideas?

In the last picture there was some “finishing” left in some places around some of the characters. What can be done to reduce this?

If someone can point me in the right directions, I will glad to search for solutions. I just don’t have the vocabulary to know what to use in my search.

Thanks,

Donnie

https://discuss-assets.s3.amazonaws.com/original/3X/5/7/5726f1bfafb1ac2e4e6155a141186a63fcf7ddee.mp4

45

02

1 Like
2

Someone that uses Easel more than I might want to chime in, but in troubleshooting for others I’ve noticed that Easel generates toolpaths that only retract to the uncarved surface rather than to a safe height. The reason I don’t say zero is because I’ve noticed it in pockets that occur within another pocket. Let’s say the surface of the S in SMITH is at Z-3.00mm, when the machine is clearing the pocket around it (maybe Z-4.5), it will sometimes only retract back to Z-3.00. If your detail bit zero isn’t perfect, you might carve a path on a travel move like that.
Can you share the Easel file?

3

Thanks for the info. I think I follow you but I’ll have to think it over before it sinks in. Here is the link:

4

First, leave the dewalt at 1. 1 is already too fast, but it works.
.1 doc is a little much for it, especially at 60ipm in my experience.
As for the finish, looks like you aren’t using a Z probe. Correct?

1 Like
5

Thanks for the info. Yes, I’m using the Triquetra and I zero’ed before the rough and the finish.

Donnie

6

The bright green (or yellow maybe?) line going right across your S, where you see the extra line in your carve, is a travel move. Travel moves aren’t supposed to cut anything. Easel has your detail bit clearing out the top corner in the S to a depth of 0.24" (why not 0.25" as in your design?..another issue?), but then it only raises to -0.125" before zipping across the face of the S to clear the random spoton the curve of the S. The surface of your S is at -0.125", so if your zero is a little off, it’ll carve on that rapid move.

image
image709Ă—458 209 KB

It’s a toolpath issue…not much to do but tell the Man that you’re carve didn’t turn out. (Or dive into hand editing the gCode…you’ll learn a ton)
As for the other things, I’d suspect a zeroing / squareness / flatness issue…probably not Easel’s fault.

7

Upgrading to the cnc4newbie z axis helped reduce this for me.

1 Like
9

Thanks Neil. Your explanation is very helpful. Another piece of info to put into memory (I’m starting to fill it up fast). The .24 question is something I noticed from time to time. It was set to .25 but sometimes I’ll notice that Easel will change a depth ever so slightly.

Thanks,

Donnie

10

Tim,

I just got the machine running during Christmas. The z axis is on my list of “future” upgrades.

Thanks,

Donnie

1 Like
11

Robert,

I’ll poke around the z axis area tonight and see if anything is loose or needs adjustment. One thing that I failed to mention is that the chatter is not present when using a smaller size bit (1/8", 1/16") at the same speeds but smaller DOC.

Thanks,

Donnie

12

Did you caliper your Triquetra? I noticed mine was slightly different than the “ideal” and used my calipered measurement instead. Charley may have fine tuned his process since I got mine around 1.5 years ago.

Your other issues are either Z probing issues or Z axis give related. Make sure everything is tightened properly.

Switching to a linear Z cleared most of my issues that were similar but also, make sure your bit is square to the waste board. A non-square bit can cause chatter. Mine is just slightly out of square in the X direction and causes some chatter issues when moving quick and deep on a carve. I still need to correct that but for the most part, it isn’t affecting my carve quality right now.

13

With the Triquetra there is a “Fine Tuning” process available. When I set mine up just measuring and ran the app to generate the Gcode but it did not yield the desired result. Close but not exactly on. I then ran through Charley’s fine tuning procedure and now it is right on the mark.

14

Thanks Justin. I checked and everything seems to be in square. Yes, I calipered the Triquetra and entered the numbers into Charley’s workbench. I think I will try re-checking it all this weekend.

Donnie

15

Thanks. I’ve done the process but I think I’m going to double check it this weekend.

Donnie

16

I sent in a help ticket to Inventables referencing this forum post. Specifically, I was wondering if they could shed some light on the “line across the S” and if there was a way to prevent this. They responded that they have had this reported recently by others and were working on a code fix to prevent this issue. They said they hopefully should have the fix in place next week.

I want to thank them for their prompt response and excellent customer service. I also want to encourage anyone that post an issue here on the forum to also send it to Inventables (if appropriate). They can’t fix issues unless they know about it.

Thanks to everyone,

Donnie