[CadRhino]

Nyccnc has a good video on YouTube using job zone. It was one of his last sc videos.

I I haven't really gotten into using the job zone to limit work. I like to use virtual fixtures to block out areas that I don't want the machining to go. I use the primitive fixture and will use negative numbers for x, y and z to partially block a workpiece. In the case of the plaque, I blocked off the English phrase with a fixture and machined the characters. Then I moved the fixture to block off the characters and machined the phrase.

R J

[Bryan Turner]

I do a lot of complex micro-engraving (0.002-0.004 tip engravers). I've had good results on gold, silver, copper, and aluminum.

Here are some general guidelines for micro-engraving:
- Use the largest tip and widest angle you can get away with to keep up the strength of the engraver (ie: 60-degree tip is better than 30-degree tip, 0.01 tip is better than 0.005 tip, etc.).
- Use ball mills when possible, they're stronger.
- Not all carbide is the same! I've used "China carbide" and Bits & Bits carbide, same size, same speeds and feeds -- Bits & Bits lasts 5 times longer.
- When you need to go narrow & deep, clear out the engraving using progressively tighter bits - start with a 60-degree, then go to 30-degree, etc.. I've gotten down to 6-degree cutters 0.03 deep with 0.004 feature sizes using this technique, this is the limit I have time for with the 770's 10k spindle.
- When you want sharp features, but don't have time for the speeds and feeds of a 0.002 engraver, use a larger tip to clear out the majority of the engraving, then use the fine tip engraver to trace the outline of the feature just a few thou deep (0.002 - 0.004 deep). Visually this will have the same impact as if the entire engraving was done with the 0.002 tip engraver. A fine eye or magnifier will see the slight shelf left by the higher resolution tip, but for most purposes this works just fine.

If you use SprutCAM, there are a few specific issues to watch for:
- The engraving operation works well for some tool geometries and just goes wonky with others. Check the cut path it generates!
- The engraving operation sometimes skips 'levels' (ie: 0.002 deep, 0.004 deep, 0.008 deep ... wait, what?).
- I often use the Pocket operation instead -- setup the tool as a cylindrical end-mill with the appropriate tip size, then program the side-angle for the engraver you're using in the pocketing op (not the tool geometry). [NOTE: my version of SprutCAM 10 will not save the side-angle parameter when using the wizard view (double clicking the op to get the parameters), I have to use the operations tabs below the operations list to set it]
- For some reason, after many tweaks and re-computes on an operation (engraving or pocketing), the tool paths start to get sharper, like the compute engine is loosing resolution every time I hit the run button. For micro-engraving this totally destroys the features. I have not found any way to correct this, even copying the op and reset/run on the new op does not fix it. The only workaround I've found is to delete the op and program it again from scratch. Works fine this way, but I have to check & re-check the generated paths to make sure it hasn't started to lose resolution.

--Bryan

[CadRhino]

This makes sense. Thank you for sharing your own insights and techniques, Bryan

I do a lot of complex micro-engraving (0.002-0.004 tip engravers). I've had good results on gold, silver, copper, and aluminum.

Here are some general guidelines for micro-engraving:
- Use the largest tip and widest angle you can get away with to keep up the strength of the engraver (ie: 60-degree tip is better than 30-degree tip, 0.01 tip is better than 0.005 tip, etc.).
- Use ball mills when possible, they're stronger.
- Not all carbide is the same! I've used "China carbide" and Bits & Bits carbide, same size, same speeds and feeds -- Bits & Bits lasts 5 times longer.
- When you need to go narrow & deep, clear out the engraving using progressively tighter bits - start with a 60-degree, then go to 30-degree, etc.. I've gotten down to 6-degree cutters 0.03 deep with 0.004 feature sizes using this technique, this is the limit I have time for with the 770's 10k spindle.
- When you want sharp features, but don't have time for the speeds and feeds of a 0.002 engraver, use a larger tip to clear out the majority of the engraving, then use the fine tip engraver to trace the outline of the feature just a few thou deep (0.002 - 0.004 deep). Visually this will have the same impact as if the entire engraving was done with the 0.002 tip engraver. A fine eye or magnifier will see the slight shelf left by the higher resolution tip, but for most purposes this works just fine.

If you use SprutCAM, there are a few specific issues to watch for:
- The engraving operation works well for some tool geometries and just goes wonky with others. Check the cut path it generates!
- The engraving operation sometimes skips 'levels' (ie: 0.002 deep, 0.004 deep, 0.008 deep ... wait, what?).
- I often use the Pocket operation instead -- setup the tool as a cylindrical end-mill with the appropriate tip size, then program the side-angle for the engraver you're using in the pocketing op (not the tool geometry). [NOTE: my version of SprutCAM 10 will not save the side-angle parameter when using the wizard view (double clicking the op to get the parameters), I have to use the operations tabs below the operations list to set it]
- For some reason, after many tweaks and re-computes on an operation (engraving or pocketing), the tool paths start to get sharper, like the compute engine is loosing resolution every time I hit the run button. For micro-engraving this totally destroys the features. I have not found any way to correct this, even copying the op and reset/run on the new op does not fix it. The only workaround I've found is to delete the op and program it again from scratch. Works fine this way, but I have to check & re-check the generated paths to make sure it hasn't started to lose resolution.

--Bryan

[Bryan Turner]

Horrible cellphone photo, but this was on the machine earlier today. 0.004 feature size, 0.02 deep using a 15-degree engraving bit in 14k rose gold for a wedding band. A quick brush on the rubber wheel removes the burrs and leaves the edges crisp. Probably fill this one with black wax for contrast since gold doesn't patina much.

--Bryan

Attachment 329380

[CadRhino]

Very nice. Thanks for the photo.
I am getting the spence that 'engraving' can be a little like 'carving'

Horrible cellphone photo, but this was on the machine earlier today. 0.004 feature size, 0.02 deep using a 15-degree engraving bit in 14k rose gold for a wedding band. A quick brush on the rubber wheel removes the burrs and leaves the edges crisp. Probably fill this one with black wax for contrast since gold doesn't patina much.

--Bryan

Attachment 329380

[CadRhino]

Thanks for everyone's input, photos and sharing our experiences. I just ran (17) letters that were 1/4" tall and it took six minutes for each run.

I just ran my first engravings and everything went great.

This is what I did;
- I used a 1/32" 4FL ball end mill off of ebay (Kyoceria)
- I messed around with creating closed polyline's in cad and finally came across this link to create text in sprutcam - Engraving on a Flat Surface – SprutCAM 9 | SprutCAM America Blog
This was helpful but I had to make some changes.
- I wanted skinny single stroke font to reduce time and width of letters so I chose Euro.chr single STROKED font from the SC text menu.
- I tried to use the Finish Engraving function but SC kept wanting to make pockets between the letters. Since I was using single stroke letters I selected everything and used 2D contouring.
- If you use SC, this method is fast., It took me 15 minutes to cam everything for the first time.
- I ran the EM at .0025" DOC, 4 IPM at 5100 RPM. I did three passes and the final DOC was .0075"

Thanks, again for all the input.

Nathan

This makes sense. Thank you for sharing your own insights and techniques, Bryan

[popspipes]

Thanks for everyone's input, photos and sharing our experiences. I just ran (17) letters that were 1/4" tall and it took six minutes for each run.

I just ran my first engravings and everything went great.

This is what I did;
- I used a 1/32" 4FL ball end mill off of ebay (Kyoceria)
- I messed around with creating closed polyline's in cad and finally came across this link to create text in sprutcam - Engraving on a Flat Surface – SprutCAM 9 | SprutCAM America Blog
This was helpful but I had to make some changes.
- I wanted skinny single stroke font to reduce time and width of letters so I chose Euro.chr single STROKED font from the SC text menu.
- I tried to use the Finish Engraving function but SC kept wanting to make pockets between the letters. Since I was using single stroke letters I selected everything and used 2D contouring.
- If you use SC, this method is fast., It took me 15 minutes to cam everything for the first time.
- I ran the EM at .0025" DOC, 4 IPM at 5100 RPM. I did three passes and the final DOC was .0075"

Thanks, again for all the input.

Nathan

Nathan, I use Rhino 4, and it has mecsoft-1 (single line font) in the text selection this really works great for me.
I also use the 2d contour for engraving, single flute engraver, 5140 at 5 ipm .010 deep in aluminum.
The fonts are a real pain, some have super imposed lines etc and various other problems.

Yesterday I used a font that I downloaded for free off the net, then used curved line with points to trace the letters, then just exported the curves as an .igs file, imported it into sprut and cut as a 2d file, worked great.
Fairly fast once you get used to it and I have my single line font from a dual line font.

I use the cheap single flute cutters, I could break a .03125 end mill by looking at it ha!!
On the other hand the four flutes means I could go 4 times faster for the same results, food for thought??

have fun, I get a kick out of engraving things..........

[CadRhino]

Very nice piece, Mike sr.
Is that an example of the wood pieces you have been machining? Nice finish.

So to sum up my experience with the first time engraving, the 1/32" 4-fl ball endmill on a36 steel had nice sharp line for the first (144) 1/4" tall letters then was not looking as sharp and created a good bur on the edges. I could still use the parts just had to debur them in a scotch brite wheel.
The first bit broke after (150) letters/2 hours of running.
a36 is not nice material to machine but I rechecked my z and it had changed by .001"
This must be due to the tormach spindle heating up. Normally for the parts I make this would be ok but on fine engraving on hard steel it wore the bit on the first plunge.
The second bit completed the remaining parts (759) letters. The last 500 weren't pretty but clear enough after scotch briting.

Aluminum would have been more forgiving.

Anyway I got my parts done and am happy.

Thanks

Nathan, I use Rhino 4, and it has mecsoft-1 (single line font) in the text selection this really works great for me.
I also use the 2d contour for engraving, single flute engraver, 5140 at 5 ipm .010 deep in aluminum.
The fonts are a real pain, some have super imposed lines etc and various other problems.

Yesterday I used a font that I downloaded for free off the net, then used curved line with points to trace the letters, then just exported the curves as an .igs file, imported it into sprut and cut as a 2d file, worked great.
Fairly fast once you get used to it and I have my single line font from a dual line font.

I use the cheap single flute cutters, I could break a .03125 end mill by looking at it ha!!
On the other hand the four flutes means I could go 4 times faster for the same results, food for thought??

have fun, I get a kick out of engraving things..........

[CadRhino]

That is good to know about rhino fonts. I use rhino sometimes.

Btw, does anyone know if the 4-fl 1/32" ball mills would also work on aluminum or do I have to go with 2-fl? I would like to only stock one cutter instead of two.

Thanks

Nathan, I use Rhino 4, and it has mecsoft-1 (single line font) in the text selection this really works great for me.
I also use the 2d contour for engraving, single flute engraver, 5140 at 5 ipm .010 deep in aluminum.
The fonts are a real pain, some have super imposed lines etc and various other problems.

Yesterday I used a font that I downloaded for free off the net, then used curved line with points to trace the letters, then just exported the curves as an .igs file, imported it into sprut and cut as a 2d file, worked great.
Fairly fast once you get used to it and I have my single line font from a dual line font.

I use the cheap single flute cutters, I could break a .03125 end mill by looking at it ha!!
On the other hand the four flutes means I could go 4 times faster for the same results, food for thought??

have fun, I get a kick out of engraving things..........

[kstrauss]

If exact depth of the engraving is not particularly critical I often set Z=0 slightly above the workpiece to reduce the impact of thickness and clamping variations. It may take slightly longer but it is worth it if it saves a cutter or having to scrap a part. Did you get your cutters from drillman1 on eBay?

[CadRhino]

No, They were kyceria brand off of eBay.
Nathan

If exact depth of the engraving is not particularly critical I often set Z=0 slightly above the workpiece to reduce the impact of thickness and clamping variations. It may take slightly longer but it is worth it if it saves a cutter or having to scrap a part. Did you get your cutters from drillman1 on eBay?

[popspipes]

Very nice piece, Mike sr.
Is that an example of the wood pieces you have been machining? Nice finish.

So to sum up my experience with the first time engraving, the 1/32" 4-fl ball endmill on a36 steel had nice sharp line for the first (144) 1/4" tall letters then was not looking as sharp and created a good bur on the edges. I could still use the parts just had to debur them in a scotch brite wheel.
The first bit broke after (150) letters/2 hours of running.
a36 is not nice material to machine but I rechecked my z and it had changed by .001"
This must be due to the tormach spindle heating up. Normally for the parts I make this would be ok but on fine engraving on hard steel it wore the bit on the first plunge.
The second bit completed the remaining parts (759) letters. The last 500 weren't pretty but clear enough after scotch briting.

Aluminum would have been more forgiving.

Anyway I got my parts done and am happy.

Thanks

Thanks Nathan for the compliment.

They are pine boxes made from 2x4 lumber, nothing special. The harder the wood the better the finish it seems.

The wood block games arent stained, I do sand them though, Over 2000 of them so far, keeps the old guy busy ha!

I dont know if you use sprut?? If you do try slowing the plunge down to about 10 to 20 percent will help the longevity of the cutters.
I personally like 3 and 4 flute cutters for everything, they seem to run quieter than a 2 flute and are more rigid.

I need more rpm for the wood products, then the finish would be better without sanding.

[CadRhino]

I do use sprutcam but am always learning. Where do you slow the plunge rate down?
Thank you

Thanks Nathan for the compliment.

They are pine boxes made from 2x4 lumber, nothing special. The harder the wood the better the finish it seems.

The wood block games arent stained, I do sand them though, Over 2000 of them so far, keeps the old guy busy ha!

I dont know if you use sprut?? If you do try slowing the plunge down to about 10 to 20 percent will help the longevity of the cutters.
I personally like 3 and 4 flute cutters for everything, they seem to run quieter than a 2 flute and are more rigid.

I need more rpm for the wood products, then the finish would be better without sanding.

[philbur]

Thanks Ray
Tormach's single flute carbide 1/8" engravers only go down to 30 deg. Do you think those will work well. I am attempting to do 14 and 18pt. Open text.

A general recommendation is that the height of the text should be 7 or more times the diameter of the cut width, and you need a depth of cut somewhere around 0.3mm. If you have a feed rate per rev (single lip cutter) that is greater than 1/2 the diameter of the cutter tip then you are guaranteed to break it. 5% feed is probably a safe number. So 14 point text at say 3.2mm high gives you a width of cut of about 0.45mm. Using a 30 degree cutter at 0.3mm doc gives you a maximum cutter tip width of approximately 0.25mm So at the 5% feed and 5000 rpm you have 62mm per minute feed rate. I guess you follow the thinking so you can apply your own numbers. If you break a cutter reduce the feed rate and try again. As you can see the larger the tip width the grater the feed rate.

I used the above principles to engrave these (from memory) 2.5mm high numbers in mild steel.



Phil

[CadRhino]

Hi Phil
Nice part and thanks for sharing your recommendations.

A general recommendation is that the height of the text should be 7 or more times the diameter of the cut width, and you need a depth of cut somewhere around 0.3mm. If you have a feed rate per rev (single lip cutter) that is greater than 1/2 the diameter of the cutter tip then you are guaranteed to break it. 5% feed is probably a safe number. So 14 point text at say 3.2mm high gives you a width of cut of about 0.45mm. Using a 30 degree cutter at 0.3mm doc gives you a maximum cutter tip width of approximately 0.25mm So at the 5% feed and 5000 rpm you have 62mm per minute feed rate. I guess you follow the thinking so you can apply your own numbers. If you break a cutter reduce the feed rate and try again. As you can see the larger the tip width the grater the feed rate.

I used the above principles to engrave these (from memory) 2.5mm high numbers in mild steel.



Phil

[popspipes]

I do use sprutcam but am always learning. Where do you slow the plunge rate down?
Thank you

parameters,speeds and feeds, check the work feed box and select approach feed, set it as a percentage of the work feed in the box below it.
If the work feed says 100% then approach should be about 10 to 20 percent. At least thats what I am comfortable with and it seems to work OK here.

edit: Sorry I took so long to answer, goverment job for the bandsaw that I am always too busy to fool with ha!

[CadRhino]

Awesome
Thanks!

parameters,speeds and feeds, check the work feed box and select approach feed, set it as a percentage of the work feed in the box below it.
If the work feed says 100% then approach should be about 10 to 20 percent. At least thats what I am comfortable with and it seems to work OK here.

edit: Sorry I took so long to answer, goverment job for the bandsaw that I am always too busy to fool with ha!

[mountaindew]

Look around in the feeds and speeds dialog as mentioned above you can set a speed for about everything and as always check code as not everything posts out to your File.
Also please post some pictures of some of your engraving results. I have not done much engrave work other then with carbide chamfer mill in alum / plastic. and its not very clean and precise but good for what I was learning and doing.

[MichaelHenry]

Look around in the feeds and speeds dialog as mentioned above you can set a speed for about everything and as always check code as not everything posts out to your File.
Also please post some pictures of some of your engraving results. I have not done much engrave work other then with carbide chamfer mill in alum / plastic. and its not very clean and precise but good for what I was learning and doing.

Here's an engraving I did in acrylic shortly after I got my mill:

Attachment 330098

The bottom is still covered with the brown protective paper and I think I used the Proxxon high-speed spindle (die grinder) at 20,000 rpm with a 1/8-in carbide, half-round engraving bit from Bits & Bits. The black coloring is engraving wax that was rubbed into the engraved markings.

[pickled]

Look around in the feeds and speeds dialog as mentioned above you can set a speed for about everything and as always check code as not everything posts out to your File.
Also please post some pictures of some of your engraving results. I have not done much engrave work other then with carbide chamfer mill in alum / plastic. and its not very clean and precise but good for what I was learning and doing.

Here was a fun one from 6 years ago. This was just using a cheap carbide 60 degree V-bit done on the 1100. Photo was taken after the first coating of Dykem was rubbed off with some acetone. It is one of a set of custom coasters made as a gift. 6061 T6 material 5,000RPM, 3.1 IPM, and 2 passes at 0.0035" each with a final 0.0015" pass to clean up.Attachment 330114