engraving question

[wildcat99]

I have block letters on a surface to engrave. I would like to make one pass, so I need to drive the centerline with a contour path. Is there an easy way to create the centerline or do I need to 'xform offset-contour' for each letter and then trim/extend, cleanup??

 

I tried the stick font, but it doesn't look as good. For one thing, the legs on the W are crowded too close together.

 

Or maybe I should stay with the block letters that I have and use a different toolpath. How does everyone else do engraving?

 

Thanks for your help!

[Matthew]

I use the MCX Box Font. This produces a center line of all the letters, then I contour chain (or window select) and then I turn compensation off so the tool will follow the center of the path and not offset to one side.

[edmBosto]

wildcat,

You can also try using a smaller carbide ballmill,

and maybe even alter the W just a tad. You can get carbide ballmills as small as .015 dia.

It all depends on the circumstances for each situation.

[New Job]

We do our engraving with center drills, but we never have to go very deep .005 to .015" to get what we need.

[Matthew]

Oh yeah, I use a ball nose end mill too. I usually use a 1/16" carbide. Only need to go .002-.005" deep, any deeper and the letters don't look very crisp.

[wildcat99]

Thanks for your help. I went back to the Drafting (stick) Font because that gives you the Drafting Options to rotate and mirror the text.

 

I also modified the W and went to a smaller ball like you suggested and it looks good on the screen! We'll see how it actually turns out. These are engraved letters .015 to .020 deep in a mold cavity, so when molded they will be raised letters on the plastic part.

 

The mold halves are cast aluminum and the machine is a 5-ax router. Probably not the ideal combination, but I think it can be done.

[Mark Baker CNC Software]

I'm not how many people are using it but there is an "Engrave Toolpath" that does a nice job with tapered cutters. The toolpath automatically calculates the centerline and will rise up in the corners to get sharp transition.

[htm01]

when lettering is big enough (1/8 +) i use a 30 deg split blank,and project a pocket toolpath of arial font,

also on alum molds and recycle logo's on becu

[edmBosto]

Mark do the letters need to be surfaces for that to work as you state?

[Mark Baker CNC Software]

The engrave toolpath only needs wireframe geometry to do a 3axis toolpath. So any of the true type fonts can be used with the toolpath. The only time that you need surfaces is if your doing a 4 or 5 axis engrave toolpath.

[edmBosto]

Thanks Mark as I didn't realize that.

[htm01]

"Engrave Toolpath" is a add-on right? you need a code to unlock

[Mark Baker CNC Software]

The engrave toolpath is an add-on. If you'd like to try it, send me some wireframe geometry and the cutter info (tapered cutters - the important info is the angle and radius)and I'll run a toolath for you. I've cut a fishing pole handle that came out really nice, I have a video if anyone would like to see it (the video isn't the best)

[ggamalski]

with block font i use modify, break, draft/line. in toolpath i use contour. window around entities. in toolpath parameters use ramp, comp off, no lead in-lead out and xy stock=0

[camgeneration]

I always use,project, 3d contour, no comp. I used a 4 sided pointy cutter, just lightly break the point with a diamond file. and go .01 to .015 deep. It leaves a real sharp clear text. I only go .0005 per pass. with a 15000rpm at 50+ipm in tool steel.

[wildcat99]

OK, I can't use a ball like I first thought. The letters need to be somewhat square-bottomed to match existing parts and need to be .05 to .06 'line' width and .016 deep. This is a one time job with 104 letters, 9/32 tall, total to cut.

 

What do you suggest for a cutter and starting feed/speed to do this on a router?

 

I'm looking at:

 

4-flute carbide miniature endmill, .050 diameter, .004 corner radius, .150 LOC, 1/8 shank and 1.5 OAL.

OR

3-flute HSS taper mill, .060 tip diameter, 1.0 LOC, 3/8 shank, 2.25 OAL with 2deg taper per side.

 

The carbide will probably give crisper letters, but I'm thinking the HSS might be more forgiving and less chance of breaking.

Thanks for your help.

[edmBosto]

You can try a 3/64 Dia. X .046 flute length carbide end mill and pocket the path. You may need to create new letters for that, but that way your cutter radii will be smaller. You can also do it with a .030 flat that way.

Probably the best choice would be to just use your 4 flute .050 cutter and contour it with no offset and step it down, but ramp entry it.

I only milled graphite, but I would think you'd need 30,000 rpm. I'd need to look at a chart on the surface speed.

[wildcat99]

I've only got 20000 rpm. The ramp is set at the default 3deg angle and looks good in backplot. I found some charts and it looks like .0005 to .001 chip load is a starting point.

 

I didn't mention this tool will be in a 3/4 x 2-in extension, so it may not be the most rigid setup.

 

With this, I'm looking at 18000rpm and 20 to 30ipm. This would drop the chip load to .0003-.0004. Too fast? Too slow?

I'm paranoid when working with these little-bitty cutters since they are so easy to snap off. Thanks for your help.

[edmBosto]

better safe than sorry since it's molding and if it breaks you may see it in the final part.

We burn our molding engraving. Your cutter is engraving steel to be molded so it's all different.

good luck

[wildcat99]

I finally got the time to cut these letters and have a problem. The first letter is a P and the straight segment seems to cut OK, but the curved part of the P doesn't go deep enough. In fact it doesn't show at all.

 

I've created a plane on the angled surface where the letters are and this is the C-plane and T-plane The WCS is set to Top, but I'm not using WSC.

 

Ramping is 3deg, default settings. Filter is set at .0001 tolerance, One-way with Arcs checked in all planes.

 

It looks perfect in Verify.

 

I might try it without ramping or filter or both.

 

Any ideas??

[DavidB]

With engarving use depth by contour this will give better tool life, always turn off lead in/out, and use filter.

[wildcat99]

Thanks, I got it done.

 

My first cut had a positive 'Depth' and this did some strange things.

 

I put in a negative depth and increased my Z origin in the program to get it to cut where I wanted.

 

I'll look at this closer tomorrow when I have time, to see why it didn't like a positive depth.

[Greg VN]

Mark you've got mail I sent you a file to take a look at when you have some time.

Thanks

[wildcat99]

I found out what's going on now. The angled, engraving surface was an existing surface, not one I machined, so I had to sneak up on it to make sure the letters didn't get too deep or fade away.

 

That is why I ended up with a positive 'depth' value, which is fine if I would have increased the 'top of stock' value by the same amount.

 

Simple stuff, but throw in some angled tool planes, ramping and changing the origin point at the last minute, it gets a little confusing. Learned something new today, so the next engraving will go much quicker.

 

BTW the engraving looks great and I didn't even break one of those little baby cutters! 20000rpm at 5 to 10ipm is what worked, maybe a little slow, but no mold repairs or hand finishing needed. Thanks for your help!

[doyleg]

still didn't answer question about getting a font that is just a stick and not a box