V-bit carving text in a single pass using ArtCam Insignia?

[jonny_apple_seed]

I have a question about cutting cursive text in a single pass. I am running ArtCAM Insignia using their v-bit option, selecting a 90 degree bit that cuts a maximum of 0.188 inches and a maximum width of about 0.2". I am using a 0.25 step down so based on what I think should happen it could cut the text in one pass. But it jumps all over the place and looks like it thinks it has to cut down one side of the text and up the other.

My current project has a run time of just over 6 hours and I believe that if I could just get it to cut in a simple pass I could cut it to under 3 hours. I am not concerned about quality as it is intended to be rather rustic. I just can't afford the 6+ hour run time.

I am running on a PRTAlpha cutting 1/2" raw MDF with a 5 HP Colombo so have no issues on depth or speed of the cut.


Help...

[joe]

Jon,

My experience with Insignia is that it will make a pass around the complete letter, no matter what.

Over the years I've never had a 6 hour cut time on V carve letters. You must be doing some detailed carving. This sounds like a 3D file.

Are you saying your 90 degree bit only has a cutting ability of .188" or is the the limits you are setting.

Please fill me in on your process.

[jonny_apple_seed]

Joe:

I have taken a high resolution image of an old document and created an EPS file in Inkscape. It was not quit that simple but that is basically how the EPS was created. I imported the EPS into Insignia and then use the v-bit option with a 90 degree bit to create the tool path. That deepest it ever cuts is 0.188" and with a step down of 0.25" it should be able to do it in a single pass. The final product is about 45"x80" with small text, hence the long run time.

I have posted the same question on ArtCam's forum but have found it lacking in user or ArtCam staff support.

I did attempt to manually clean out the code by running an "air cut" and marking each duplicate pass but after about 2 hours my estimate was it would take about 80 more hours to complete. Not really an option.

I'm afraid you are right and there is not much I can do about it. I was just hoping someone has figured out a work-around to this problem.

Thanks for any input...

[ron_varela]

Jon
I am 100% positive that if you sent me the picture you did in high resolution I can make it cut in less then 22.5 minutes in 2d
If it is in 2 1/2 d it will cut in 29.6 minutes.
If it is in 3d it will take 36.4 hours.
If the letters are wider then the v bit than you are looking at .13 hours per letter with a 1 inch letter.
If you are doing it grayscale you are looking at 37.6 hours for the same size.
There is no 2d file that you can draw that will take more then 46.7 minutes with 746 cuts on a 4x8, on a 5x10 will take 48.3 minutes per 2.7 letters per line at 6 letters the same width.

Ron

[ron_varela]

PS: Inkscape to a eps is a bad move period.

[joe]

Jon,

Now I understand what you're doing. My experience with small or deliclate V carveing over a large area is how important it is to have an absolutely flat carveing surface. This might require a re-surfaceing first.

I'd take Ron up on his assistance. He's given me some excelent help in the past and really knows his stuff. If he says he can do it, He Can. This chap know his stuff. I have to agree with him about your conversion to eps.

I must agree with you about ArtCam Forum. It's close to being a dead duck.

[jonny_apple_seed]

Ron: I have not counted each and every letter but my estimate is that I am cutting just over 7,000 letters and punctuation in 2 ½ d, all cursive. Not in my wildest dreams (or nightmares) could I ever imagine cutting this in those time frames. This project was an exclusive never to be cut again order for a client. My real goal in all this is to learn how to do something like this better and faster.

If you don’t mind me asking why so down on Inkscape? I have found it to be extremely useful on hundreds of projects. What do you use or recommend?

Joe: You are correct. I re-surface the table any time I cut something like this. Nothing worse that a long run only to cut it up and throw it in the bin. Same question to you about Inkscape. What would you or do you use.

The old adage that if you give a man a fish he will eat for a day but if you teach him to fish he will eat for a lifetime really holds true for me. So if there is a way I would rather learn how to do it rather than have someone do it for me.

[ernie_balch]

Jon,
Your project is suffering from data overload, just how big is a file that takes 6 hrs to run?

Inkscape is a good program for vectorizing but it can leave you with thousands of points per character. This will really slow down the router.

You can do the job with brute force and experience long cutting times or you can find some way to filter out a lot of the extra data points without distorting your text.

[scottcox]

Jon,

Check out Vector Magic at http://vectormagic.stanford.edu/ .

It does much better than any other raster to vector converter I've used. I can't speak for Inkscape because I've never tried it.

Vector Magic does have a file size limitation, but other than that, it's very functional. It's the only program I've used that doesn't produce extensive pixelization of the edges.

I'm guessing that could be a cause of the long run times. When you v-carve a pixelated edge, it treats every little zig-zag as a "corner", coming back to clean it up.

Also, some fonts carve very differently. On my shopbot, the Engraver font seems to take at least twice as long as others.

Just throwing my two cents in there. Good luck.

[rnels]

Jon,

Are you questioning the order in which ArtCAM cuts the text? It sounds like you are wondering why it jumps around so much when cutting. I have ArtCAM Pro so I don't know what features you have in Insignia but under the V bit carving option in Pro there is a drop down field called sequencing. When you drop this down there are two options allowing you to select the type of processing you want. One of these options is Auto and has a box to the left that says optimise. If you drop this list down one of the options is use text order. Not sure if that is what you are looking for or not.

[ron_varela]

Jon
What is the width of the letters at its widest point?

[knight_toolworks]

sounds like investing in a larger vbit would save you quite a bit of time.

[ron_varela]

Jon is this what your trying to do?


8324

8325

This is easy to do if you have the right bit.
I think the pictures are from my good buddy Joe Crumley

[ron_varela]

Jon had some free time so I ran a test on the 7000 letters and it took 53.4 seconds to cut the word SAMPLE in cursive.
The width of the letters were 1.0 inch and 7 inches high and 13 inches long with a speed of 2.0
To do this type of carving in a single pass you will need to have a v bit that matches the width of the letter, if your letter is ¾ wide then a ¾ v bit will work, or you can use any other v bit wider then ¾ diameter.
Now if you only have say a ¾ bit you can trick any software into thinking the bit is bigger, you just make a new tool in the tool database and make it like this
If the letters are say 1 inch wide and you only have a ¾ v bit make a new tool with 1.0 diameter with a depth of .25 and save it with a new name and select that tool to make the tool path.
Now just zero the bit to your material and run the file, the letters will only be ¾ inch wide at the widest point of the letters and taper off on the top.

Everyone has their own comment on what is the best raster to vector program and Inkscape is good for something’s but not everything, everyone is looking for the Holy Grail, that one program that will do it all.
My 2 cents is if it works for you great, if not try others that will.

Just do the math on the time listed above to see how long it will take to cut 7000 letters, the longer the bit is on the table the less time to engrave them.
If you are able to preview your work do that first, if you like it cut it.

Ron

[jonny_apple_seed]

Ernie: I have broken it up into 6 separate files and call them one at a time so I don’t think there is data overload. I think you are right and that Inkscape is probably not giving me nice clean edges which could account for a lot of the run time. That and the original hand written text is not nice and crisp either.

Scott: Thanks for the link and the tip on fonts running faster or slower than others. I will have to give Vector Magic a try.

Randy: Insignia does let you select Top to Bottom or Right to left ect. Sounds like the same in Pro. Which I could afford the jump.

Steve: I program it by selecting a 1.25” 90 degree v-bit. With a maximum depth of cut at 0.188”, my widest cut is 0.376”. With the 1.25” 90 degree v-bit I should be able to cut 0.625” deep which would be cutting through my sheet and into the bed. I actually only run with a 1” 90 degree v-bit but neither the machine nor the software know that I cheated.

Ron: That is basically what I am doing although the actual text was originally hand written and is not nearly as clean and crisp as what you posted. I am doing very similar cuts to what you have in your pictures, but still have the same problem with those. I have a scroll cut I run frequently and will email it to you in .dxf, .art and the .sbp formats if that is okay with you. It does the same double pass that I don’t need and would like to try and eliminate. Wouldn’t be able to email them until I get back to the shop on Monday.

I am ever amazed at the input I see and now experience first hand on the ShopBot forum. I am glad there was never enough money to jump into the “big time” CNC world. I do some molder work for a shop next door and do not envy their monthly payments. I would rather have 10 ShopBots rather than the one they have.

[ron_varela]

Sure Jon send me the files and I will look at them.

Ron

[john_l]

I have used a guy named Eric... netsearch "The Vector Doctor". Send him junk raster and you get back great vector, minimum points. I have been using node editing software for many years and I still find it way better to pay this guy $10-20 to take care of something that would take us an hour or two to do. Not affiliated, just a suggestion.

[joe]

Jon,

I stand to be corrected, but I don't think any 2.5 D V Carve programs are designed to make cuts in a single pass. If it's done in one storke, the corners won't be crisp, just rounded. I'm sure your are close to finding a much faster, cleaner path for this project.

Like you, I've used Insignia for years but all my prep work is done in Flexi Sign Pro. Their scanning program is very good but again pricey. Most scanned art has a minimum amount of nodes. I hear the new Corel X3 is a top contender in the scanning business also.

Ron. Thanks for the reminder

I'd almost forgoten about the Waterford project. It was one of my first attemps with Insignia. That was years before V Carve Pro came on the scene.

[Call-Tech]

Jon,

I too have been fighting with ArtCam's Vcarve. I assume that there is just something I don't know about it. It seems to always want to cut deeper than I believe it should. And if you limit its depth, then artcam does not make one pass down the center line and cut narrower, it makes multiple passes inside each letter until the proper width is achieved.

I have never posted a photo so I don't know if this will work, but here is a photo of some vcarving I was testing to try to get around this irritating feature in artcam. this photo is out of ArtCam and shows the multiple passes it creates when you limit depth while using V carve. And your right about it jumping all over the place. It's cut order seems completely stupid. ArtCam is such a great software, but I am constantly fighting its auto, optimized order.


8326

I'm not trying to hijack your thread, I think we are asking the same questions and I am looking for help also on V carving with Artcam.

I find that if I use the simple little text cut program that is embedded in my shopbot 3 software. I can cut perfect V carved Text. If I try to do the same font, same size Text in ArtCam, then it is too deep, takes much longer and does not look anywhere near as good.

Any Idea what I'm doing wrong?

Sincerely, Fred

[Brady Watson]

Jon,
It appears that VCarve Pro or ShopBot PartWorks2D will do Vcarving in a single pass as long as you have the stepdown large enough. I only tried a few letters and carefully viewed them in the SB Previewer to watch each move. You may want to give that a try.

Hand-digitized vectors are ALWAYS better quality than any raster to vector conversion software. There are many people who can do this for you for a fee or use one of the resources mentioned in this thread.

--

Fred,
I think you'll get better results in ArtCAM if you make some modifications to your current parameters. Understand that Vcarving takes the Vee of the bit and only goes as deep as the point where the sides of the Vbit intersect 2 lines. |V| This is why a 60° bit will cut deeper than a 120° bit - and incidentally the proper way to control depth is with the angle of the bit. From your posted pic, it appears that you have your stepover value too large (showing stepover marks) and your tolerance may be too low. You should specify a tolerance of .0005 for Vcarving in ArtCAM. Try experimenting with larger bits for larger letters and designs. The smaller bits will cut deeper, and the only way to control this and still get a prismatic look is to alter the angle of the bit.

Here's a general V-Bit Angle Recipe (http://www.talkshopbot.com/forum/messages/315/15365.html?1159827619#POST40966) that I came up with. It isn't set in stone, but it is a good starting point.

-B

[jhall]

Jon,
My suggestion would be to use a program such as Coreldraw to re-type the copy in the correct ( or as close as you can get it ) font. You can then position and size as needed. This would give you a very "clean" vector file to use.
A lot better than a trace or convert and a ton better than doing it by hand.

Terri

[joe]

I think Jon is using a scan because he wants to reproduce a specific affect. By setting copy you revert back to a more mechanical look.

Brady,

Are you sure about the single pass? I don't think its possible in 2.5 D.

John,

Since Jon is making such a shallow cut I don't believe there is a much of a consideration for a tool limit. If this were my job however, I condiser a 120 degree bit since it makes small lettes read better.

[ron_varela]

Joe they got off track and are talking about artcam now

[frankwilliams]

I may be out of line, but postprocessor selection could affect file size(cut time) if you are not using the arcs processor. Probably nothing to it, but the thought occured so I thought I would throw in my two cents.

[joe]

Ron,

I've tried ArtCam Pro and ArtCam Insignia but can't see any difference if using the 2.5 stategy. I believe they are identical for this strategy. Over the years I've used Rams, Insignia, V Carve Pro and ArtCam Pro. It's a flip of a coin which is best. They all start up on the inside on a letter, one side at at time, lifting up the the intersections. Even a simple "O" with equal sides it takes two strokes.

As usual I stand to be corrected but a single stroke strategy doesn't produce a very attaractive letters since the corners are rounded.

[Brady Watson]

It sure looks like it does it in one pass to me...but then again the SB Previewer on my computer runs a little fast in simulation mode. See for yourself. Generated in VCP.

The downside to single stroke v-carving is that the tool doesn't come back to cleanup the letter. So in reality, you have one side of the vee climb milling and another conventional cutting. This is why most v-carving engines double back to do a cleanup pass.

-B




8327 (8.5 k)

[jonny_apple_seed]

Brady: Thanks for the file. It looks like it does a partial double cut but I have not run it on my Bot.

I sent a few files over to Ron and he took a look at what I was doing. As far as I can tell in order to get clean 2.5 d v-bit carving this has to be some double cutting.

I also got a response from ArtCam staff on their forum. He said "you are trying to apply the V-Bit Carving toolpath to a closed loop, currently there is no way/control to apply the toolpath within one pass."

He did say there is "already an existing wish(development task) to have V-Bit Carving with single pass for closed loops/vectors".

So it sounds like it may be a future option from ArtCam.

Thanks for everyone's input.

Jon