Need Help! First attempt at engraving - Page 3


Page 3 of 3 FirstFirst 123
Results 41 to 60 of 60

Thread: First attempt at engraving

  1. #41
    Registered
    Join Date
    Aug 2009
    Location
    USA
    Posts
    106
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    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

    Last edited by Bryan Turner; 08-02-2016 at 12:46 PM.


  2. #42
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

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

    Quote Originally Posted by Bryan Turner View Post
    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




  3. #43
    Registered
    Join Date
    Aug 2009
    Location
    USA
    Posts
    106
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    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

    First attempt at engraving-img_3411-jpg



  4. #44
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

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


    Quote Originally Posted by Bryan Turner View Post
    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

    First attempt at engraving-img_3411-jpg




  5. #45
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    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



    Quote Originally Posted by CadRhino View Post
    This makes sense. Thank you for sharing your own insights and techniques, Bryan




  6. #46
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by CadRhino View Post
    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..........

    Attached Thumbnails Attached Thumbnails First attempt at engraving-kaylas-boxes-png  
    Last edited by popspipes; 08-06-2016 at 03:19 PM.
    mike sr


  7. #47
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

    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



    Quote Originally Posted by popspipes View Post
    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..........




  8. #48
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

    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

    Quote Originally Posted by popspipes View Post
    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..........




  9. #49
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1788
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    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?



  10. #50
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

    No, They were kyceria brand off of eBay.
    Nathan

    Quote Originally Posted by kstrauss View Post
    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?




  11. #51
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by CadRhino View Post
    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.

    mike sr


  12. #52
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

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



    Quote Originally Posted by popspipes View Post
    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.




  13. #53
    Gold Member
    Join Date
    Jun 2006
    Location
    Suffolk, UK
    Posts
    2512
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by CadRhino View Post
    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

    Last edited by philbur; 08-07-2016 at 08:22 PM. Reason: add ref to single lip cutter


  14. #54
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

    Hi Phil
    Nice part and thanks for sharing your recommendations.

    Quote Originally Posted by philbur View Post
    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


    Last edited by CadRhino; 08-07-2016 at 11:20 PM.


  15. #55
    Member popspipes's Avatar
    Join Date
    Jun 2014
    Location
    United States
    Posts
    1777
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by CadRhino View Post
    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!



    Attached Thumbnails Attached Thumbnails First attempt at engraving-bandsaw-impeller-png  
    mike sr


  16. #56
    Member
    Join Date
    Aug 2013
    Posts
    980
    Downloads
    0
    Uploads
    0

    Default

    Awesome
    Thanks!


    Quote Originally Posted by popspipes View Post
    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!





  17. #57
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    2151
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    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.



  18. #58
    Gold Member MichaelHenry's Avatar
    Join Date
    Jun 2006
    Location
    Chicago suburbs
    Posts
    3063
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by mountaindew View Post
    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:

    First attempt at engraving-logoengravetestfinal-jpg

    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.



  19. #59
    Registered
    Join Date
    Aug 2009
    Location
    USA
    Posts
    610
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    Quote Originally Posted by mountaindew View Post
    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.First attempt at engraving-celtic-cross-coaster-jpg



  20. #60
    Registered
    Join Date
    Aug 2009
    Location
    USA
    Posts
    610
    Downloads
    0
    Uploads
    0

    Default Re: First attempt at engraving

    That's pretty cool! My Proxxon is still running strong. They are a pretty nice little rotary tool, but I rarely use it on the Tormach because I forget about it. Maybe I should move that heavy old chunk of cast iron off that bottom shelf (next to the dusty duality lathe) and put it to work LOL!



Page 3 of 3 FirstFirst 123

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

First attempt at engraving

First attempt at engraving