I've been testing out the engraving aspect of v22 and have come up against
poor quality cuts and poor resolution of the letters.
The final step in the engraving properties edit is the diameter of the cutter.
The mill drill endmill I'm using has a tip that is .03 wide at the minor diameter and tapers to .375 @ 60 degrees.
If I select a .01 depth of cut I get very poor quality cuts. (see attached photos)
In many cases there is material left that should be removed creating
islands inside the letters.
Is there a way to compensate for this? A true engraving cutter is also tapered and I assume would create the same issue.
Is it a font scale issue perhaps?

It appears to be tool related, poor cut quality, possible Dull Tool. Spacing between the outer cut and the inner cut is related to the settings you are using. It is doing exactly what you are asking it to do. It also appears your machine may not be holding tolerances very well try scaling down a thenth or so and see if that helps if your cutter is carbide try speeding it up. slow down feed speeds a bit, use new tool or sharp tool. Deflection of the tool or material could also be a factor.

Bobby,
The tool is very sharp and there is no noticeable deflection. The tip of the tapered tool is .030" wide, 2 flute. The D.O.C. I input was .01", The second part was aluminum and the speed parameter BCC set in the post was 10,000 rpm. My machine has a top speed of 4500 rpm so that is the speed the cutter ran. I have to check the cad file and see if the width of the top line of text is less than .03" wide.
I also need to check the width of the bottom text and see if it is less than .06The tool path runs twice for each of the larger letters. If there were more options within BobCad Cam cutter parameters for a tapered engraving tool, in this case minor diameter .03" and major diameter .375" with a L.O.C. of .187 then perhaps the simulator would run with a more accurate cut path.

What type of cutters do you use to engrave with BCC v22 and what is a typical DOC that you usually select?

A mill/drill really isn't the greatest engraver. Try www.harveytool.com or http://www.endmill.com/ They provide better tools for engraving. If you want to engrave a Font Outline I would suggest creating the font then pocketing the inside with a small step over.

BTW: do not try to use the start point option in the pocketing, it isn't working properly yet.;)

Cheers:)

Toby,
Thanks for the tips, I just got the Harvey catalog and am going to order a few different engraving tips.
I am going to try an inside pocket tool path this time and I'm certain that it will turn out much better.
I'll post the results.
Best, Dave

Cool!!! be sure to post those results. Though I have no real pictures (customer confidentiality) you can look at this one on my website. I have to break out the camera soon to update the site more, LOL, it's looking pretty lame.

http://www.axiscncprogramming.com/108.html

Toby,

The results for the true font engraving were improved by the 2D pocket suggestion however there are still tool path problems that must be a cutter diameter issue (see attached) The B's and R's have a part that does not mill or else it's an over cut into the negative space. I'm still not clear how the tapered cutter path is assigned since variations of DOC will result in wider or narrower cuts depending on depth. There is no major-minor diameter choice in the cutting tool parameters. The images attached were made with a .25" mill drill 60 deg. cutter.
(I am waiting on my order of Harvey cutters) Why would this occur?

Toby,

The results for the true font engraving were improved by the 2D pocket suggestion however there are still tool path problems that must be a cutter diameter issue (see attached) The B's and R's have a part that does not mill or else it's an over cut into the negative space. I'm still not clear how the tapered cutter path is assigned since variations of DOC will result in wider or narrower cuts depending on depth. There is no major-minor diameter choice in the cutting tool parameters. The images attached were made with a .25" mill drill 60 deg. cutter.
(I am waiting on my order of Harvey cutters) Why would this occur?

Well, first off I do not think your doing anything wrong. It is probably a bug in BCC and the fact that there isn't a parameter setting for Tapered End Mills.

Have you tried limiting your step over using only the tool tip as the diameter?

try a ball mill like 1/32.

I'll second HMB's ball mill idea. I've been using a .030 flat end mill on acrylic, with the Bobcad Helv font and it's working great. Tried the tapered cutter, but it was doing more melting than cutting. Same deal with speed; BC says 10K and best I can do is about 5K. I just keep it slow.

Randy and HMB,
I will try the ball end mill, thanks. The font within BCC is all well and good, however if
a client provides a 2D CAD file compatable with BCC then the CAM in this case BCC should follow it if the parameters are set up properly. Toby suggested there may be a bug with the program. I hope that this is not the case.

. Toby suggested there may be a bug with the program.

using an ingraving bit for a pocket routine is kind of buggie in itself. It not uncommon when people can't get the results they want to just say it a bug.
Even thou someone else sends you a font file you need to look close at it. as with some fonts the chained geomitry is sometime junk

If I understand correctly the chained geometry in question is the combination of straight lines and arcs found in all letters.
If a font's geometry is "junk" how is this determined?
If a tool path error occurs it could be either be a bad font or a bad CAM reading or I guess even a post processor error. In addition it could also be a poor cutter or a poorly chosen cutter.
Therefore:
Question: when does one use a tapered engraving tool vs. any other tool and how does one determine .ttf compatibility?

using an ingraving bit for a pocket routine is kind of buggie in itself. It not uncommon when people can't get the results they want to just say it a bug.
Even thou someone else sends you a font file you need to look close at it. as with some fonts the chained geomitry is sometime junk

That is funny but after some research there is a bug. This bug really isn't a bug with BCC. It is a bug in Microsoft Fonts. Seeing that I spend most of my time dealing with parts not engraving I asked a good friend about Fonts and their reaction to CAM software. He informed me of some fonts are better while others are buggy when doing any type of engraving.

I suggest you use a different font or clean the geometry of the font after Vectorization before posting your code.

brooklynmetal,

It looks to me like you are using a Windows font. Is that true? If it is then this explains the cuts you are getting with the Engraving option.

Because the font, when vectorized, is a profile of the letter you have a path on both sides. This is why you have the islands in the center of the letters. The Engraving option is designed so that you can create a centerline cut using the defined geometry. It is not a Pocket style toolpath.

For Windows fonts you are going to want to use a Pocket Toolpath not an Engraving type. This will confine the tool to the inside of the letters you are trying to cut.

Regards

That is funny but after some research there is a bug. This bug really isn't a bug with BCC. It is a bug in Microsoft Fonts. Seeing that I spend most of my time dealing with parts not engraving I asked a good friend about Fonts and their reaction to CAM software. He informed me of some fonts are better while others are buggy when doing any type of engraving.

I suggest you use a different font or clean the geometry of the font after Vectorization before posting your code.
Toby,
Thanks, I will check to see what I did with the differant tests I ran.
I did not use Bob Art but imported type layout as 2D .dwg file into BCC.
I will try a small ball end mill and use a Window font as a pocket and test it out.

brooklynmetal,

It looks to me like you are using a Windows font. Is that true? If it is then this explains the cuts you are getting with the Engraving option.

Because the font, when vectorized, is a profile of the letter you have a path on both sides. This is why you have the islands in the center of the letters. The Engraving option is designed so that you can create a centerline cut using the defined geometry. It is not a Pocket style toolpath.

For Windows fonts you are going to want to use a Pocket Toolpath not an Engraving type. This will confine the tool to the inside of the letters you are trying to cut.

Regards
The One,

Thanks, I tried using a Corel and Word type layout with Bob Art V22 but it was going to be a huge amount of work to clean up the type. Next I took a 2D .dwg text layout in full scale and imported it into BCC. Wouldnt this .dwg file already be a vector file? I will have to check and see if I created an engraving path or a pocket tool path. I will set up some new tests. The CNC requires a lot of time and patience but it is very enjoyable. Best

brooklynmetal,

If you imported a DWG file with text in it, then it may be a vector file. The problem here is that when you vectorize Windows Fonts, you get an outline of the letter, just the edges. So it is not a centerline representation of the text, which is likely what you are looking for with the information you have posted so far.

When you generate an Engraving Feature for this geometry, you will have the tool cutting centered on the line. This is how you end up with those areas that are left standing.

A pocket might take a little more effort to make sure that your depth and step over are what you are after, but it shouldn't leave the areas in the center raised as it has in your previous postings.

Regards

Well I have use a 60deg engraving tool for finish path across the entire surface with good luck. Here is the coin I did.
I have also used them for other 3d work of a customers part needing fine detail on acrylic.

because of the parameter of the cutter is not correct

Well I have use a 60deg engraving tool for finish path across the entire surface with good luck. Here is the coin I did.
I have also used them for other 3d work of a customers part needing fine detail on acrylic.

Very nice coin cadcam. Excellent Detail!!!!!!:rainfro: Using fine point engraving tools always work for applications such as this.

What version of MC did you use and does it have the Art Add-On?

Well I have use a 60deg engraving tool for finish path across the entire surface with good luck. Here is the coin I did.
I have also used them for other 3d work of a customers part needing fine detail on acrylic.

yes you did a very nice job. right tool for the right job. But I still use ball mills for pocket type fonts. I will use an ingraving bit for stick font.

HMB I do both. of course it matters on the aplacation kind of like the coin. this was done with two tools, the one I spoke of and the other a 1/16 ball for roughing.