Engraving help

[Adrian]

How are you setting the z-zero? Still looks like the z-zero is too low to me if you're sure the bit matches the specs you've entered.

[martin54]

As was said earlier it looks like a problem with your z zero setting, you said in one of your posts that you were using a mat to hold the material, I am wondering if you are compressing that mat when setting your z zero which will give you a false zero position

If you are not getting what the toolpath preview is showing then the problem almost certainly lies with the machine or it's control software

After you set your z zero position how ever you do that try going back to your zero position & checking that the bit is not set to low

[Truck trudeau]

I hear what you’re saying about the z depth but I’m not so sure. If I engrave more shallow I still get the same problem. I don’t think it’s going deep enough for the angle to be the reason why the letters are so wide. I feel like if there was no angle it would look the same. I’m going to do some at .001 and .002 today. I actually have an engraving bit (parallel cutter) with no angle I’m going to give that a shot as well. I find my Z with paper as I find it to be more accurate than the plate. the mat is perfectly flat, strong and literally does not move even when plating there is zero flex. It’s what the engraving shops use when they are rotary engraving this plastic. If you’ve never heard of a multi mat before check it out it’s like 500 bucks for 24“ x 24“ but it works amazing. The entire plastic sheet stock that I’m using has a high-end 3M 2 sided tape backing. After engraving when I cut out the profile of the shape I can cut exactly through the plastic without hitting the adhesive part of the backing tape anywhere on the bed of the machine that’s how accurate the machine and z axis seem to be. I’ll attach the text version of the tool paths later today. Thanks again for the help!

[Truck trudeau]

I should also mention that when I scale it way up so the letters are 2 inches tall each I still get the same problem. So if a small letter was 1/32 too wide a big letter might be 1/8 too wide. Same depth. I’m going to try this again today to confirm as well

[Adrian]

I hear what you’re saying about the z depth but I’m not so sure. If I engrave more shallow I still get the same problem.

You're misunderstanding. It's not the z depth that is being queried it's the z-zero setting on the machine. If that isn't correct it doesn't matter what you set the z-depth to as the starting point will be wrong so cutting shallower won't change anything.

[Truck trudeau]

Maybe I’m misunderstanding…. I set Z to zero by using a piece of paper and slowly jogging the machine down until the paper stops moving. it’s accurate to the .0005 but correct me if I’m wrong. I find by using the plate it can be out by as much as .0015. If I can cut out a profile in plastic that is exactly 1/16 and I set the depth to .0625 and it cuts exactly through the material without leaving a mark on the mat underneath. Do you still think I’m misunderstanding? I just want to make sure I’m being clear. Thanks!

[Adrian]

Well if you're confident your z-zero is accurate it's going to be the tool definition or flex on the machine or movement on the material. People are cutting jobs like this every day without issues so it's not a problem with VCarve especially as the toolpath preview for the job you posted is spot on (v-carve top, quick engrave bottom in the attached pic).

Everything you're showing in the pictures is a tool that is cutting too deep or is not the tool that v-carve has been programmed with for what I can see.

I would try a piece of material with the adhesive removed and place it directly on the spoil board rather than the mat. That's how I work with material like that and have zero issues. Trouble shooting problems like this is all about removing as many variables as possible and then changing one thing at a time until you crack it.

[Truck trudeau]

Thanks all for the help. The problem seems to be the depth and the angle of the bit. If I engrave at .002 it just barely makes it through the color and the text is closer to the correct yhickness. At .001 it just scratches the surface. So I don’t know how the experts do it but seems I need a flat bottom bit with flat sides for the first .005 or so otherwise it’s all too wide…. Vcarve is calculating based on the flat part of the bit even though some of the bevel comes into play…. I guess it doesn’t come up often enough but some sort of “v depth offset” setting in vcarve or parameter that based on depth makes thing thinner if you know what I mean would be great. Thanks again for all the help and I’ll post pics once perfectly dialed. Last problem is that the machine seems to vibrate at times but I’m thinking that’s just a lubrication issue…. Hopefully…. Thanks again!!

[adze_cnc]

and the text is closer to the correct thickness

A blanket statement: VCarve is consistently behaving as it was created to do so. Any deviation you are seeing in the physical results on the material is due to other factors (either at the machine or a mental model of how things should work in conflict with how the program does work).

The following image shows the 2D view in VCarve with the preview of three toolpaths (top to bottom):

1. "Quick Engraving Toolpath". Using your 30 deg side angle and 0.015 flat bit. Instead of "Fill" I used "Outline". Both options will produce this result. "Fill" just adds the internal clearing that obscures what I want to point out.
2. "V-Carve / Engraving Toolpath". Using your 30 degree side angle and 0.015 flat bit.
3. "V-Carve / Engraving Toolpath". Using a 60 degree incldued angle v-bit (30 degree side angle)

The first two toolpaths are directly from your file. The third I added myself. The "Quick Engraving Toolpath" does look "thicker" but there is a reason for that.
 

Three toolpaths mentioned in the above list

 
The "Quick Engraving Toolpath" is generally used with a spring-loaded pointed scratching tool so the "Depth / Pressure" is merely how much to compress the spring. With a cutting router bit it will be the depth of cut (akin to the flat depth in the "V-Carve / Engraving Toolpath".

The toolpath can accept v-bits or engraving bits. But these may not behave as people want them to. But they do behave in a predictable fashion.

A "Quick Engraving Toolpath" using a flat-bottomed engraving tool such as you are using will always producde "thicker" objects than a "V-Carve / Engraving Toolpath". When the toolpath runs around the outline vector it does to "on the line". So really a "Quick Engraving Toolpath" using the "Fill" option is a combination of a "Pocket Toolpath" combined with a "Profile Toolpath" running "on the line".
 

Engraving bit can't quite get into the tip of the A because it is a truncated cone

 
A "V-Carve / Engraving Toolpath" will never cut outside the lines. So, the objects cut with this toolpath will always (at least in the theortically perfect software preview) never be "thicker".

As I mentioned in a previous reply the only difference between using a v-bit (theortically pointy) versus an engraving bit (with a flat) in a "V-Carve /Engraving Toolpath" is that the corners will be a little softer with the engraving bit. The following two images show that. In the first one the engraving bit can't quite get into the corners to make things fully sharp.
 

Quick Engraving shows the engraving bit riding on the line making the shape larger than "it should be"

 

V-bit can get into the corner because it is a "true" cone

 
It really is unfortunate that Vectric chooses to use a "T" as the icon for "Quick Engraving" as this leads people into believing that if they are doing something text-based that this is the best toolpath to use. If you are using a spring-loaded diamond-tipped scratch tool on glass, metal, acrylic, stone, etc. then yes it is useful for text. If you are using a v-shaped router bit then the "V-Carve / Engraving Toolpath" (unfortunately named as it confuses with the product name and the quick engraving toolpath) is probably a much better choice.

So, I'd say unless there is a specific need to use the "Quick Engraving Toolpath" stick to the "V-Carve / Engraving Toolpath". The only quick engraves I've ever done were on copper plates to be used with intaglio printmaking and those used a diamond scratch bit.

[Truck trudeau]

Thank you very much for that very detailed reply it makes sense. As soon as I get a chance to get back to the machine I’ll be back on here I still have a few more issues. Thanks again!!

[adze_cnc]

Erratum:

Photo captions: "Engraving bit can't quite get into the tip of the A because it is a truncated cone" and "Quick Engraving shows the engraving bit riding on the line making the shape larger than "it should be" " need to be reversed.

[Truck trudeau]

thanks again for the detailed post and all of the help! Well the more hours I spend on this machine the more I learn that’s for sure. I had no idea about the residence and the significant amount of time the industry has spent trying to fix that problem. So this is where I’m at with engraving plastic. If I do a job with the quick engrave toolpath The lines may be a tad bit thicker than they should be but I get A+ quality of engraving. I can do it at 100 in./min. and most of the lines are crisp and perfect. For some reason when I use the vcarve toolpath with a flat depth I get terrible quality. Have a look at the attached pictures. That was done at 20 inches per min. Does not matter how slow I go the edges are terrible and it seems like it’s too thin even?? Like the bit was supposed to go back around but it didn’t maybe?? I don’t know…. So at first I was thinking that had to do with resonance but it does not happen nearly as bad with quick engrave. Very strange.

So it doesn’t matter if it’s text or a logo if I use quick engrave I get oversized engraving but the quality is great. If I use v carve tool path I get like in the attached picture…. Yes the text is small but again it does not happen with the Quick engrave toolpath. Any suggestions about that? Also I should mention that when I use the vcarve toolpath if I turn on the clearance tab it creates 2 toolpath‘s but even after running both of those two paths it misses parts of the job. It does so on the preview as well. I hope there’s some setting or something stupid that I’m doing because this is starting to make me crazy…. Thanks again for all the help!!

[martin54]

There is something else going on here, you shouldn't get edges like that using the vcarve toolpath, are you using the same text for both quick engrave & Vcarve/engraving toolpath?
I know you said engravers use the mat you use but most engraving machines also use a nose cone which helps keep the material flat & stops it moving,
I can't help thinking that some of those bad edges may be caused by material movement.

[Adrian]

The sample file you provided early showed a perfect preview but now you're saying that the preview is missing parts out?

The picture looks like a cut done with an endmill not a v-bit. It's 100% something you're doing wrong rather than a problem with the software otherwise the forum would be full of people with the same problem but where you're going wrong is hard to figure out at the moment.

Can you attach the file that shows missing parts in the preview

[adze_cnc]

Your images are not captioned. To clarify: the “ELEC” one was done with a V-Carve toolpath? The “1-855” one was done with a quick engrave toolpath?

If the “1-855” is indeed a quick engrave then I’d say it suffers from the same malady as “ELEC” one. Look at the 2nd and 3rd “www” especially. The edges are in no way smooth and straight. The only reason it doesn’t manifest as much is in using the rastering hatch option.

If you run a quick engrave on the “ELEC” but use the offset instead of the hatch option I’d expect a similar result to the V-Carve toolpath.

I’m surprised nobody has suggested: is your machine trammed properly?