ShopBot Problems Continue

[Steve Wonser]

I had been having problems with my ShopBot Desktop slowing down and then stopping in the middle of a cut. I disabled USB power management and that seemed to go away. However, now the it seems like the ShopBot is loosing the X position.

I was engraving an acrylic piece using a spring loaded 90 degree diamond drag bit with the spindle off and no dust collection attached. The job ran for 1:35:05 without stopping. The attached pictures show the following problems:
- The hatched area is not consistent. The acrylic is not flat (0.002 difference from the thinner left side to the right), but the spring loaded bit should take care of that. I set z-zero to the top of the acrylic. The engrave depth/pressure setting is 0.01 and the fill stepover is 0.004. Feed speed is 1.4 inches/second.
- There are vertical lines in hatched areas that should not be there.
- After the ShopBot finishes hatching an area it outlines the perimeter. It is clear in the pictures that the outline on the right has move about 1/8" to the right.

Any ideas as to what is happening and what I might do to fix it?

Thanks,
Steve

[Tim Lucas]

looks like an off set on the outline?

[steve_g]

Steve…
Just to be sure you know… You can choose whether or not to have that last profile pass. See photo.
What I’m seeing Appears to be a loss of steps. That would account for the perimeter being offset one direction, it could also account for some of the inconsistency. Also, I’m wondering if the hatching started from one direction, went to the opposite end of the area and started coming back the opposite direction. That scenario would be the perfect storm of all accuracy issues working against you!
SG

[scottp55]

Steve, Is it rastering along the Y axis starting on the left and going to right?
Safe Z and Z2 settings are?
Are "Bubbles" cut last or first? Are "Bubbles" clean?
Am I not seeing it in pic or is the Tail and beginning of S pretty good?
Is Drag tool mounted IN spindle collet, or in an offset mount?
scott

[Brady Watson]

It appears to me that the depth of the drag in certain areas could have been too deep for the tool to be able to drag it - and it lost steps. This would be indicative of the offset on the profile you see to the right of the main part. Acrylic is 'catchy' and it would not be hard for it to really create some resistance against movement - especially during short, quick moves.

Diamond drag tools are typically not used to create the effect you show here. Nothing wrong with it - just that it isn't a very efficient strategy. You could create the same effect with less 'whiting' using a 1/32 or 1/16" end mill or tip-off engraving tool with the spindle running.

'Engraving' as it relates to using a diamond drag or engraving tool usually involves what they call centerline engraving using single stroke fonts and line art, much like a Profile-On toolpath with a tool at a fixed depth; or a quick engrave toolpath with cross-hatching to create a fill. It usually isn't done with such a fine tool to clear out a big area.

I don't mention any of this to be critical - just as information.

-B

[scottp55]

Brady, ZERO acrylic experience, But lots of guys on Vectric site doing edge lits similar to this.
I was just wondering, IF Steve is Y rastering and the stepover was SLIGHTLY too close, AND there was ANY play in insert...Would acrylic try to pull it back into the previous groove? Then it might be twice? as deep, and as Z isn't lifting could it be causing missed steps.
My age is showing, but even with the lightest stylus pressure on Vinyl records, once a "skip" started, it got harder and harder to jump "Out of the Groove".
I was wondering if acrylic and diamond drag Y rastering would cause the lost steps, trying to force its way out of a 2-3 time cut groove.
Doug or Jeff, has it ever happened to you?
Should be following "Bradys Rule" "If you don't know...Stop talking and Listen!"
Jus' Cain't seem to help Ma se'f:)

[Steve Wonser]

It is rastering along the Y-axis starting at the head of the fish and moving to the left. When it got to the far left it outlines the fish parts. The bubbles were done last after the outline. The bubbles look like they came out correct except for being shifted to the right.

The drag bit is in a 1/4" collet, but there has to be some slop in the bit because it is spring loaded. I haven't attempted to measure it.

The way that there are missing vertical lines would seem to follow Scott's theory that the bit is getting stuck in a previous groove then pops out and moves to where it should be leaving a blank spot. This is also inline with Brady's observation that the grooves may be too deep.

After popping out of the groove it seems like the X-axis would be back on track. What does it take for the steppers to loose steps?

I've attached pictures of my settings.

[Steve Wonser]

I just looked at the settings pictures that I posted. I can't read them. Sorry about that. I'll try again tonight when I get home.

[Steve Wonser]

I converted them from PNG to JPG to see if that makes a difference.

[Brady Watson]

Hey Steve - Your settings look fine.

Question - Is there any reason you are not machining with a rotary tool, such as an engraving bit (Micro100 makes nice stuff) for this work? I think you will get better & more reliable results, especially on a 1.5hr file.

-B

[Steve Wonser]

Brady, I really new to this stuff. I saw the acrylic etching done on this and on the Vectric forums and after much reading I came to the conclusion that people really liked using the diamond drag bits.

I'm open to any and all suggestions that will help me to get better at this. I'm not familiar with a rotary tool. Can you provide more information? You're right it does seem crazy for this to take 1.5 hours.

[Brady Watson]

By 'rotary tool' - I mean an engraving bit, such as those sold by HarveyTool (http://www.harveytool.com/) or Micro100; or a small end mill, say 1/32" from same said manufacturers. These would be used with the router spinning.

You are going to find that end mills are going to be your go to tool for most things. They are the same grind as 'upcut spiral' bits, usually cheaper @ higher tolerance and better quality. Solid carbide only, unless messing with aluminum.

I'm unclear on your desired finish for this example. If it were me, and I needed to clear out those big areas, I would use a pocket toolpath. However the machining marks may or may not be desired - raster angle is important. Avoid 'offset' pocket machining or it will look goofy. I would then follow up with a Profile On strategy with a v-bit, engraving bit or small end mill to do all of the single stroke 'engraving' around each perimeter.

Again, I am not sure what your overall intentions are with the piece, so it is hard to advise you in greater depth. If you aren't sure - that's OK too. There's lots of learning to be had messing about - as you are finding out.

Here's a little something (http://www.talkshopbot.com/forum/showthread.php?t=4719) I worked on about 10 years ago on my 5x16' Bot. I used a ball end mill at first, then switched to a proper engraving bit (Micro100) for the remainder of the guilloche pattern. Better results are to be had on a Desktop due to improvements in electronics and mechanical resolution compared to the machine this was made on...I'm just making you aware of what is possible...which aught to stir the juices a little.

-B

[POPS 64]

Steve , I'll send you a pm ,see if I can help . Jeff

[Steve Wonser]

Brady thanks for the info on the rotary tools. I'll have to give it a try sometime. Your work in aluminum is pretty amazing. Those designs would look great in edge lit acrylic.

[Brady Watson]

Thanks Steve.

What one man can do, another can do... (http://youtu.be/9ALOI63X_CE) ;)

-B

[Steve Wonser]

I gave it another try last night. I didn't want to change too many parameters so I loosened the spring on the dragbit and did the Z-Zero using Jeff's method for that bit.

The good news is that it didn't loose X position this time. There are still some strange differences, dark and lighter areas, in the cut quality. The attached picture shows what I mean. But it finished and the piece should be usable.

There was one strange thing that happened. About mid way through the cut the spindle started moving very very slowly. Probably like about 1/8" per second. It never stopped, but would have taken forever to finish. So I hit the spacebar to stop it, waited a few minutes while I tried to figure out whether to restart it or quit and use the goto line feature. I decided to try the restart button. Luckily that fixed it and it completed the rest of the job at full speed. Anyone know what may have happened?