[camtd]

Hi

When I create text and exploded it to engrave the number 6 does not cut all
the way.

What is the best text to use for a clean looking engraving? This is only
to identify tool numbers nothing fancy. Where the number 6 cuts all the way also.

Thank You

[miljnor]

I don't know surfcam but if you are talking about not engraving once in the machine, it is often a too high a feed rate for the machine to cut an accurate tool path (usually do to corner rounding settings or ramp up settings in the machine)

if its inside the cam interface you'll have to have someone else help you out.

[camtd]

Hi

I am talking about in surfcam itself. The toolpath this is just simple text engraving. The speeds and feeds are not the problem in this case.

Thank You

[lakeside]

with surfcam you can import almost any font I use bitstream font navigator

[scubanick]

i have the same problem with the 6 in surfcam
if u trim the loop by like .005 on the left sdie where it meets the rest of the 6
it will continue on around
surfcam has a problem or will not allow tool paths to cross unless forced with vectors
i would just trim that part of the 6 and it will work

[moldcore]

When engraving single stroke fonts with Surfcam, some of the default 2Axis Options settings have to be changed. Set the Maximum Feed Between to 0.0000, Gouge Check set to "single" and it helps to set the Sort Type to "none". Hope this helps. Don't forget to reset the default when finished.

[FatChips]

I have had similar problems with engraveing in surfcam.
I found that if you select the text/numbers useing the chain option it works best.
For the number six I select the top 'tail' then the round part.
I've also had troubles with numbers 4, 8, and 9.


Setting the gouge check to single (per moldcores suggestion) seemed to work as well. The you can just auto select the text.

[chronon1]

Is surfcam an expensive package ?
Is there any other simple text to .gc or .dxf convertors available ?

[moldcore]

Setting the gouge check to single (per moldcores suggestion) seemed to work as well. The you can just auto select the text.

Auto selecting text is the only way. We do engraving almost daily, sometimes hundreds of letters at a time. I would never think of chaining each letter or number. Using the settings mentioned above gives us error free results. Of course that only works on single stroke or line fonts, like Surfcam's default, that we use most of the time. We have a CAD program that has an add-on program that makes smooth rounded fonts and fonts where each letter is defined by two lines about .005 apart so you can pocket or profile around them leaving them raised.

Engraving is just one of many areas where Surfcam could use a lot of improvements

[Paul G. Swartz]

Surfcam doesn't allow a cutter path to run into itself with the default settings. The "2-axis options" tab has a field "Gouge Check" with a default setting of "Path Only". Any letter or number that has a branch point (4, 6, 8, 9, etc.) will be incomplete. I usually change the color of part of the letter or number, then create one tool path with the mask turned on for that color only and auto select the text. Then I create a second tool path for the remaining geometry with the other color selected in the mask. It's a tedious task but failsafe. I've played around with the gouge check settings with limited success on version 2002.