Text engraving on plastic problem

[vireo44]

I am producuing small (7" by 3") signs on plastic (white surface and black inner material). I am using Vcarve Pro 6.5, the basic Shark, and a 30 degree, 0.005" tip engaving bit. The font I am using (Arial TTF) has what I am calling "dog biscuit ends" at the end of each letter - as if the bit is routing a litle bit beyond the path. So I am ending up with whath looks like a serif font instead of sans serif. The dot over an " i " looks 2 fat lines in an X pattern. The material is 0.125 plastic and the flat depth is 0.07".

Any suggestions would be appreciated. I'd send an image but my camera won't focus close enough.

dave

[tonydude]

Can you upload the file so we can take a look at it.

Tony

[vireo44]

tonydude,

Sure, the file is attached. Thanks-

dave

[jeb2cav]

Which post-processor are you using?

[Eagle55]

can you upload the .crv file. I'm not sure I know how to look at the tap. I'm guessing that the bit angle that you are using may not match what you are telling the program you are using, but that is a guess at this point.

Roger

[tmerrill]

Dave,

If the snip below is similar to what you are seeing, that is caused by having a v-bit whose angle is smaller than what the toolpath was calculated for. In this case, the toolpath was calculated for a 30 degree bit but simulated with a 29 degree bit.

You should double check your settings in the Tool Database but the most likely cause is the bit has not be accurately sharpened to the correct angle. This is common and you can find a quick technique here to figure how what angle the bit is cutting at:

http://www.vectric.com/forum/viewtopic.php?f=3&t=2164

Once you figure out the angle and adjust the tool database to show it, then recalculate the toolpath and it should look fine.

Tim

[jeb2cav]

I agree with Tim, however I think there are 2 possible causes and that's why I asked what post processor you were using. For fine lettering, lithographs, pockets/boxes/square things, I'd recommend you use the CNCShark-USB_NewArcs vice the CNCShark-USB_3dContour post processor.

The NewArcs PP has a smaller machining tolerance than the 3dContour PP. A discussion of this can be found in the 'CNC Shark Post Processors - 3 Jan 11.pdf' available on the NWA download page.

[vireo44]

Thanks everyone for your suggestions, I have not had a chance to try any of them yet but hope to tomorrow.

The v-carve file is attached. The post processor I have been exporting to is CNCShark-USB Arcs (inch)

Dave

[Eagle55]

I know this may sound a little offensive because it is so basic, but the way I understand it you say you have a 30 degree bit. Did you specify 15 degrees in the box when you set up the tool in the database? For engraving bits it wants the "side angle" which is half of the actual bit angle. ie putting 30 degrees would actually mean the program would be calculating for a 60 degree tool bit. Its not the same as setting up a v-bit where you would put the actual tool angle. I'm not trying to insult you because it is so simple but that is a mistake that I would make LOL

Roger

[tmerrill]

Hi Dave,

Roger is correct and you need to change your tool database for that bit to show a 15 degree side angle.

I assume the attached picture shows what you are seeing? This was your toolpaths simulated with the correct setup bit. Change it to 15 degrees, recalculate the toolpath and you should be good to go.

Tim