Please Help -- VCarve and Advanced VCarve

[GeorgeMM (George)]

I thought my journey was going OK, but I appear to be in a maze of twisty passages, all alike.

I am back on my problem from months ago on the topic of small text. After much research I thought I had a good handle on an approach — and this evening the approach crashed into a bottomless hole.

I am using the Zniko font … not quite a single line font, but it should be close enough. I have set up test programs with a variety of bits, different font spacing, different font heights, different depths, different toolpaths, etc. After many runs, I thought I had a handle on how things are working. My last run took that all away.

The Zniko font has been giving me the best results. Font heights I have settled on now range between .25 and .4 inches. Font spacing of 120% looks good. Cutting depths are being tested in the range of .04, .05, .06 and .07 inches.

I am aware the VCarve will automatically select the proper depth (based on the letter width and V-bit angle) as long as you specify bottom or near bottom for the stock depth. No problems there. BUT, I was under the assumption (based on research) that if I use an Advanced VCarve by selecting a pocket end mill tool (say 1/4 inch) that is bigger than will fit, that endmill will not be used but the V-bit will carve to the depth specified since the endmill and Vee bit would need to be at the same cutting depth. That did NOT happen. The pocket carve portion came up as EMPTY TOOL (as expected), but the depth of the V-bit did NOT go as deep as expected. In fact, all the depths turned out the same. It seems now that if the pocket cut is NOT valid, that the carve defaults to a regular vcarve. I need the Vee bit to go to my specified depth! How do I do that in an advanced vcarve?

I also tried a contour path (no offset) with 30 degree vbit and while the depths did change, the results were not satisfactory. I have also tried a 1/16 straight bit but that bit was too fat. I am hesitant to go to 1/32 straight bit due to breakage concerns.

In my latest test, I also tried the 60 degree V-bit again with an advanced vcarve, and the depths did slightly change, which is really strange since I would have expected the 60 degree bit to not find a depth deeper than the 30 degree bit.

Can someone please explain to be where my understanding of using an end mill too big in an advanced vcarve will NOT allow me to specify a specific depth of cut. And my understanding of vcarve and advaced vcarve is leading me astray?

Thank for your assistance.

George

[mhotchin (Michael Hotchin)]

V Carve is the wrong approach here. Fundamentally, a VCarve varies the depth in order to place the V bit between the vector lines - the vectors are the constraint, the depth is the variable used to meet that constraint. When a depth is specified for a V Carve, it is an upper limit, it’s not the depth of the carve. Anything that would carve shallower than that is unaffected. Part of the problem here is poor terminology.

Even if you somehow could force the depth, then what result would you expect? The final result would look worse and worse the narrower the original design was. A v bit with a forced depth means every feature carved has a minimum width, unrelated to the deign.

You want the depth to be the constraint. So, contours or pockets, using endmills (since they don’t vary width with depth).

[GeorgeMM (George)]

Correct. That much I aware of for VCarves. I may not have been clear in my post, but right now I am only concerned with small text.

If I was using an Advanced Vcarve to carve a pocket in a regular design, my understanding is that I would use both a flat end mill plus a v-bit, and that the depth that I would specify is the depth that would be used for BOTH cutting operations to keep them aligned. To try to force a specific v-bit depth, I used advanced vcarve with both a flat endmill plus the vee bit at a specific depth. But in my case where the flat endmill was too large for the pocket cut, carbide create appears to neglect my specific depth of cut. I have seen other users specify their cuts in this fashion. I will revisit them again.

I have used a 1/16 bit in a regular contour cut, but there was too much tear-out in the small font. I was hoping that the pointy end of the v-bit would work better as opposed to a 1/32 or smaller bit.

I will be retesting the 30 degree bit as a contour cut with shallower depths next.

I am still confused on why an advanced vcarve is not working as expected.

Thanks for your response!

[SDGuy (Anthony)]

@GeorgeMM

Can someone please explain to be where my understanding of using an end mill too big in an advanced vcarve will NOT allow me to specify a specific depth of cut. And my understanding of vcarve and advaced vcarve is leading me astray?

If the Vector width is narrower than the EM width, the program will not cut anything. In this imag,e the Rectangle has a width of .2 and the EM is .25. The end mill will not cut anything because it can’t “fit” within the bounds of the Vector.

A V-Carve only uses a V-bit to carve the pocket. IE, no flat bottom.
Take a look at the vectors below. The toolpath for 1 is an advanced V-Carve, but since the vector is narrower than the EM, the EM is ignored. Toolpath 2 is a regular V-Carve, with a narrow Vector; everything turns out just fine. Now Vector 3 and 4 are 2" x 2". This is where the V carve vs the Advanced V carve can be seen. #3 is a regular V-Carve. Notice the toolpaths and compare them to #4, which is the Advanced V-Carve.

Simulation:

Vector #5 is the .2 x 4" Vector using a Pocket cut and a .25 EM. Notice the toolpath says “Empty”

V carve vs Advanced V Carve.c2d (104 KB)

[SDGuy (Anthony)]

Can you post your file so we can take a look?

[SDGuy (Anthony)]

I ran the Font with a 15-degree v-bit, and it turned out good.

[GeorgeMM (George)]

Thanks Anthony … I agree 100% with what you posted … and that much I do understand. I am getting EMPTY TOOLPATHs … I was expecting that.

Let’s look at your #4 above. In that Advanced VCarve, both the flat endmill (for the pocket cut) and the V-bit cut should have the same depth. Correct? Otherwise there will be lines on the bottom. Now assuming that they DO have the same depth that I specifed in the toolpath, then IF I create an Advanced Vcarve with too big a bit (ie, an EMPTY TOOLPATH results), then WHY does the Depth that I specify in the Advanced VCarve gets IGNORED for the V-bit portion! That is where my concern is. The V-bit bottom point and the flat mill should be at the same depth. But if the flat cut gives an EMPTY TOOLPATH then WHY is the VBit cut appear to revert to a simple Vcarve.

Maybe I need to try this in V7 when VCarve and Adv VCarve were separate toolpaths to see if something happened in v8.

Thanks again.

[GeorgeMM (George)]

OK … based on the comments here which got me thinking more, I have reached the following conclusions:

1. This works the same way in both v7 and v8.
2. My basic premise is not correct, and my understanding of Advanced VCarve in my situation leaves a bit to be desired.
3. For Advanced Vcarve, it appears that setting a depth will ONLY work if the pocket toolpath is not empty. If it is empty, Advanced Vcarve reverts to Vcarve functionality in most cases for a large setting for max depth. The font I used, while giving some small text does not allow a v-bit to go deeper than the vector segment width, hence the reason why all the different max depths were the same.
4. For larger text and an Advanced VCarve, if one specifies a wider flat mill, then you can specify a specific depth AND have the V-bit create the flat bottom for you without needing the flat mill. This may be advantageous in certain situations. But it will NOT allow you to specify a specific depth for thin vectors or text.
5. I need to get some 1/32 inch bits long with a 15 degree v-bit for experimentation.

Thanks again all for your comments.

PS … feel free to let me know if I made any mistakes in my above
conclusions.

[WillAdams (William Adams (Carbide 3D))]

No, the Advanced V carve algorithm (cutting around perimeter) is used regardless of the state of the pocket or lack thereof.

[mhotchin (Michael Hotchin)]

For bits remember that metric is also an option. Lots of bits available on 1/8" shanks.

1/16" is about 1.6mm, 1/32" about 0.8mm. I use 1.0mm a lot for small text. I’m mostly on wood, so I use downcut bits a lot.

[SDGuy (Anthony)]

@GeorgeMM

Let’s look at your #4 above. In Advanced VCarve, both the flat-endmill (for the pocket cut) and the V-bit cut should have the same depth. Correct?

Correct.

@GeorgeMM

WHY does the Depth that I specify in the Advanced VCarve gets IGNORED for the V-bit portion!

The max depth should be the same regardless of whether the EM is too wide to fit in the vector. To verify this, you can use the same V-bit as your clearance tool. BTW, you will get a little warning that the V-bit produces an inefficient toolpath, just click “ok”.

@GeorgeMM

But if the flat cut gives an EMPTY TOOLPATH then WHY is the VBit cut appear to revert to a simple Vcarve.

That should not happen. Here is a screenshot of a .24-wide vector and an advanced V-Carve; the toolpaths are for the 15-degree v-bit.

I have both V7 and V8. I have not run into the problem you are describing. I use V7 to do my design work, but I prefer V8 for sending to CM.

[Bozo (Bozo T Clown)]

A font very close to a single line font like Znika is unlikely to benefit from using a Vcarve or Advanced Vcarve tool path when used for small text. As you have discovered, the depth of cut becomes extremely shallow regardless of the vbit used. So… don’t do that.

To get usable depth and reasonable results with small text you have two main options:

• a contour tool path where you define your depth, use a very small bit (1/32) and a font very close to a single line font like Znika
• a Vcarve tool path (not an Advanced V carve tool path) with a 30 degree or less vbit and not use a font close to or equal to a single line font

A third less favorable option would be to use a contour tool path where you define your depth, use a very small Vbit and a font very close to a single line font like Znika. A simulation of this option would not reflect the true cut so trial and error at the machine would be necessary and the shallower the depth of cut you use, the narrower the letter strokes become, and at some point too shallow for use.Cheers.

[GeorgeMM (George)]

Bozo … I think you are right on the money here. VCarve and Advanced VCarve are not good solutions. The depth of cut was definitely too shallow with no way to make it deeper. I did try a Contour tool path with a 1/16 bit, but discovered that even that was too big. I also tried a Contour tool path with the 30 degree VBit, but that was also unsatisfactory. A 30 degree VBit with other fonts also were not too good.

My next set of tests will be to use a 1/32 or 1mm bit with the Contour tool path with the Zniko font. I am just concerned that these small bits are just going to break.

Thanks again to you and others here. I’ve spent 3 hours this morning analyzing the responses here and playing more with the simulator.

[WillAdams (William Adams (Carbide 3D))]

See:

Alternatives to single-line fonts

One work-around for a single-stroke font is to inset the text. Given a text in a font which is close to being mono-line: [image] convert the text to curves: [image] Draw in geometry at the narrowest point: [image] And then inset: [image] [image] Apply [image] and then apply a No Offset Contour toolpath: [image] [image] Attached as a v7 file carbide3d_single_stroke_alternative.c2d (140 KB)

[GeorgeMM (George)]

Will … I have seen you post that many, many times … unfortunately some of the steps go beyond my experience with Carbide Create at this time … another way for me to say this is that I’m not smart enough with CC to understand the detailed steps.

I can write the text … I can convert the text to curves (I assume you group the vectors?) … I don’t know what you mean by “Draw in geometry at the narrowest point” … once i understand what that means I can try setting the inset … but right now I am stuck.

Thanks.

[ksymons (Ken Symons)]

I’ve used the SpeTool 1/32" downcut endmill many times with the Zinko font with good results. As you’ve said, you may have to increase the spacing on the text (like 110% to 120%) depending on the letters in your text. Also, your concern about breakage is a valid one with an endmill this small. I had one break when it hit a knot in some cherry and another one break when I wacked the tip of the endmill when replacing the sweepy dust collector so you have to be careful. Since it’s a downcut bit, it works pretty well with Oramask too which I also use often.

Here’s a link to the endmill from Amazon:

https://www.amazon.com/dp/B0CTMJXVYS?ref_=ppx_hzsearch_conn_dt_b_fed_asin_title_5

[GeorgeMM (George)]

Ken … I put that one in my cart yesterday! $23 a pop … I already have the SpeTool 1/8 and 1/4 downcut bits and really like them so far. Have you tried any of the less expensive varieties? Glad to hear that it works well with the Oramask too!

Thanks.

[WillAdams (William Adams (Carbide 3D))]

Draw in a circle at the narrowest region:

Basically, keep increasing the inset until things break up — when that happens, back off.

Or, start with a too large inset, and reduce until it results in a solid/continuous interior line.

[ksymons (Ken Symons)]

I haven’t tried any other vendors for the 1/32" endmill. As long as you’re more careful when removing or putting the Sweepy back on than I was, you’ll be fine.

[Ed.E (Ed)]

Another thought on the V-Carve approach. Rather than a Start Depth of 0.00 try a Start Depth of something slightly under the top of stock like 0.025