\r\n Ger, I’m still struggling with getting Vcarve text on a 3D model. \nHere is what I did line by line, but I think I missed something as the cut depth is always way too deep. \n1. I unzipped the file you sent me. \n2. Then imported the United zipped file and aligned it on the screen. \n3. Imported the JPG of the Chinese Characters CC \n4. Went to trace bit map and placed it on the 3D material, and resized it \n5. Then clicked on the CC vectors highlighting it. \n6. Clicked Toolbars. \n7. Then V-Carve \n8. Set flat depth to 0.020” \n9. Selected 60 deg V bit and speeds \n10. Clicked on “Project tool path onto 3D model” \n11. Gave it a name \n12. Click calculate, reset preview, then preview. It all looks OK \n13. Saved toolpath to file. \nI then loaded the toolpath file into the CNC Mach3 \n1. Set XY axis to center of crown on material and lowered the Z axis until I just touched the material and set the Mach Axis to all Zero. \n2. Pressed start run. \n3. Instead of cutting 0.020” into the material it cut about 0.060” into the material. \n \nMy problem is the V bit is cutting deeper than the 0.020” in input into the flat depth. \n \nI talked to a fellow at the wood store here and he said that the 3D model and Vcut depth have to set from a different screen but he wasn’t sure how. Modeling Setup, but I cannot find that screen is it in VCP??? \n \nSorry to bug you and hope this isn’t too difficult for you \nThanks \nHager\r\n
\r\n Ger. \r\nThink I\'m trying to do something that isn\'t possible or I am not doing it properly. \r\n \r\nThe image I have is made to be cut inside the lines, but if I try and use a 0.060" bull nose bit I don\'t get the option to "PROJECT TOOLPATH ONTO 3D MODEL". \r\n \r\nIf I select a 60 deg V bit i doo have the option to project it. \r\n \r\nI would like to use the bull nose bit, is there a way ti project it onto the surface? \r\n \r\nOr what\'s a work around? \r\n \r\nThanks\r\n
\r\n Sorry for the confusion. \r\nIf i put a dim like 0.020 as the flat depth it generated dots all over the cut preview area.. \r\n \r\nif I dont put and dim in the flat depth the preview looks a solid black, and the cut depth is way to deep, set the Z zero. I zet the Z axis zero 0.060" above the surface and it makes a cut aproximately 0.020" deep which looks good. \r\n \r\nHow are you supposed to set the depth of cut on a 3D surface? i can make it look OK but im missing something in the setup. \r\nthanks \r\n \r\nphoto of preview with dots as described above.\r\n
\r\n For V-carving you need to use conical bits, even in Aspire you can project tool path onto the model if you use ordinary ball nose bit, see attached pictures. \r\nOn all simulation pictures Flat depth was set to 0.1" \r\n \r\nBall nose 0.06" \r\nAttachment 451476 \r\n \r\nConical ball nose 8 degrees, tip radius 0.00984252" \r\nAttachment 451478 \r\n \r\nV bit 60 degrees \r\n\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
\r\n If the ballnose bit is smaller then the space between your lines, than you need a flat depth to limit the depth of cut. \n \nWith a ballnose bit, you would generally want the flat depth to be at least half the diameter, or slightly deeper. Somewhere between .030-.045. \n \nIf that\'s the simulation preview, there\'s a setting for the quality. I keep mine set to the highest quality preview.\r\n
\r\n I’m missing something in setting the Vbit cut depth. \nI have a 3D shape that was sent to me, I cut it out, then move the Vbit to the surface of the material and zero the Z axis. I clicked on the characters I wanted to cut into the surface and set the flat to 000 as I had seen others do, and clicked on the follow the contour. \nI then cut the characters and they were very deep cutting into each other. Then moved the router off the object and moved the Vbit to the current Z zero, then raised the Vbit 0.060” and set Z zero at that height, (0.060” above the material) and cut the text into the material, this time the depth was OK. \nI’m not understanding how the Z cut depth is set, will I have to make this type of compensation each time I apply text to a 3D surface? \nI must be missing something, can’t believe VCP would have to be ran like this.\r\n
\r\n You can not set flat depth to 0. \nIn V-carving process, flat depth is just what it says, a level under which cutter will not plunge deeper. \nStarting depth is depth at which your geometry will follow your drawing boundary. \nFlat depth is the final depth that the cutter will descend to. \n \nSo, with the model that Gerry attached, I set flat depth for both cutters in the linked video to 0.1", Start depth at 0 and VCarving was projected to the underlying model. \nDon\'t be confused with finishing operation near the end of the video, it is just for cosmetic purposes stock has to be machined to the shape of the model \n \nhttps://youtu.be/TIg5uwQ9810 \n \nIn any case, please read the documentation for the software that you use.\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
\r\n Your Z zero is in the wrong place. \nThe g-code is only cutting between .02 and .03 deep. \nAfter it finishes cutting too deep, jog the Z axis down to the surface, and see what the DRO is displaying?\r\n
\r\n GER, \nIt’s difficult to tell the Z depth but it looks like 0.040” from the material surface. \nG code cutting between 0.020” and 0.030”. That’s should be about right because it’s cutting on a 3D radius of about 3”, and The cut width across the radius is 0.700” \nWhat do you mean my Z is in the wrong place? \n \nThe finish cutting will be on a wooden sword where the radius is about 3”. The Z zero setting will be made from the surface of the sword and 0.020” deep. \n \nHager\r\n
Your Z zero is in the wrong place. \nThe g-code is only cutting between .02 and .03 deep. \nAfter it finishes cutting too deep, jog the Z axis down to the surface, and see what the DRO is displaying?
\r\n \r\n
\r\n
\r\n
GER, what do you mean my Z is in the wrong place, could you give me some more details on that and where the Z should be. \nThanks \nHager\r\n
\r\n Your code is perfectly fine, as Gerry also noted. \nSomething with your Z zero might be wrong. \n \nBTW what are your tool offsets? Your code is calling for one: \n \n
\r\n
\r\n
\r\n \r\n \r\n N140 G00 G43 Z0.8000 H1\r\n \r\n
\r\n
\r\n
\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
Your code is perfectly fine, as Gerry also noted. \nSomething with your Z zero might be wrong. \n \nBTW what are your tool offsets? Your code is calling for one:
\r\n \r\n
\r\n
\r\n
Zasto. \nOffsets, I have never used offsets on the CNC. Is that something that is associated with cutting on a 3D surface? \n \nSomething wrong on the Z? that was the first thing I checked with a indicator, the travel over one inch was off less than 0.001”. \n \nMy friend wants me to Vcarve his Chinese name (characters) on the surface of his wooden training sword. The sword cost $65.00 and I’ve got one shot to do it right. I have Vcarve hundreds of flat signs and never had this kind of depth issue, but then this is my first try at cutting on an existing 3D surface.\r\n
You need to set Z zero so the tip of the tool is just touching the wood at the high point.
\r\n \r\n
\r\n
\r\n
Thanks for responding GER, yes that’s where I trying to describe where I set it. \r\nZasto said that I was using a Z offset, I’ve never knowingly used an offset. Is that’s what causing it to cut deeper than 0.020”? \r\n \r\nI’m just about ready to give up setting a Z depth the way I have (and how Vectric says to) for years and set the Z axis zero 0.020” above the surface in order to have the V cut be 0.020” into the surface. But I’m kinda afraid to because I’ve got one shot to Vcut my friends sword, and don’t want to spoil it. \r\n \r\nLooking closely at the bottom of the V cut it is not making a clean V cut, it seems to be cutting on each side of the Vector but not running in the center to clean that area out. \r\nDo you know why this is happening? I and setting the V depth to a flat bottom of 0.020”.\r\n
\r\n As I wrote, your G-code is using an offset: \r\n \r\nN140 G00 G43 Z0.8000 H1 <- added spaces for readability \r\nN140G00G43Z0.8000H1 \r\n \r\nSecond, from your image it looks that you are using ball nose bit, not V bit as the code was generated for. \r\n \r\nThis are the comment lines at the beginning of your G-code: \r\n \r\n( CHINESE NAME 650 20 deep ) \r\n( File created: Monday November 02 2020 - 08:21 AM) \r\n( for Mach2/3 from Vectric ) \r\n( Material Size) \r\n( X= 10.000, Y= 10.000, Z= 1.000) \r\n() \r\n(Toolpaths used in this file \r\n(CHINESE NAME 650 20 deep) \r\n(Tools used in this file: ) \r\n(1 = V-Bit {60 deg 0.625"}) \r\n \r\nCheck in Mach 3 for Height offset for tool #1\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
As I wrote, your G-code is using an offset: \n \nN140 G00 G43 Z0.8000 H1 <- added spaces for readability \nN140G00G43Z0.8000H1 \n \nSecond, from your image it looks that you are using ball nose bit, not V bit as the code was generated for. \n \nThis are the comment lines at the beginning of your G-code: \n \n( CHINESE NAME 650 20 deep ) \n( File created: Monday November 02 2020 - 08:21 AM) \n( for Mach2/3 from Vectric ) \n( Material Size) \n( X= 10.000, Y= 10.000, Z= 1.000) \n() \n(Toolpaths used in this file \n(CHINESE NAME 650 20 deep) \n(Tools used in this file: ) \n(1 = V-Bit {60 deg 0.625"}) \n \nCheck in Mach 3 for Height offset for tool #1
\r\n \r\n
\r\n
\r\n
As I said before I haven’t intentionally added an offset, I have never used an offset in 10 plus years. I have no idea how it got there. \nWhat does that offset do? \nDo I need to just delete that offset line? \n \nYes it is a V bit not a ball nose. \n \nYou say check in Mach3 for height offset for tool no 1. I looked in Mach3 and the table looks exactly like the one you posted above. \n \nAny suggestions? \n \nThanks for taking the time to respond \nHager\r\n
\r\n Ok, the offending line that is calling for offset is in post processor. \r\nJust edited it and reformatted a bit. \r\n \r\nPlace the post processor file in: c:\\Program Data\\Vectric\\...\\V8.5\\My_PostP\\ \r\n... identifies your software, I use Aspire \r\n \r\nAnd, attach your Chinese graphics that you created so that I can try to make a simulation \r\n \r\nRename the extension of this file from .txt to .pp\r\n
\r\n \r\n \r\n 3. Instead of cutting 0.020” into the material it cut about 0.060” into the material. \n \nMy problem is the V bit is cutting deeper than the 0.020” in input into the flat depth.\r\n \r\n
\r\n
\r\n
Watch the Z axis DRO while it\'s cutting, and you should see that it never goes deeper than about .038". \nBecause of the curved surface, the depth will be .020 at the highest point (center), and get deeper as it goes down the curve to maintain a constant depth of .02. \n \nIf you are testing on flat material, it will be cutting twice as deep at the edges, but you won\'t see that on the curved surface. \n \nThe g-code does not go deeper than .038-.039", so if it\'s cutting deeper, either the machine is losing steps, or the Z zero is set incorrectly.\r\n
Ok, the offending line that is calling for offset is in post processor. \r\nJust edited it and reformatted a bit. \r\n \r\nPlace the post processor file in: c:\\Program Data\\Vectric\\...\\V8.5\\My_PostP\\ \r\n... identifies your software, I use Aspire \r\n \r\nAnd, attach your Chinese graphics that you created so that I can try to make a simulation \r\n \r\nRename the extension of this file from .txt to .pp
\r\n \r\n
\r\n
\r\n
Here is the Chinese name in a Jpg format hope that will work for you\r\n
\r\n If there is no length value in the tool table, then the tool length offset is not the problem. \nIt\'s included in every vectric post processor, and it\'s likely been in every g-code file you\'ve ever created in V Carve Pro. So again, probably not the problem.\r\n
\r\n From your picture, it looks that you have some parameters wrong in tool settings in Aspire. \r\nYour step over is too big and your depth of cut is shallow. \r\n \r\nI can replicate the artifacts that are visible on your photograph only if I set depth to 0.05" and step overs as per attached image.\r\n
\r\n Could we have an image of your tool?I suspect it may not have a sharp point.I have tried engraving with such a tool and it didn\'t work too well,so I bought a small range of engraving tools that did come to a sharp point and it helped a lot.The big giveaway was that attempting to engrave a font with serifs had a zone in the serifs that went outside the outline of the lettering;in this case there are no serifs but the absence of a sharply defined line at the bottom of each symbol seems to be a clue.\r\n
Could we have an image of your tool?I suspect it may not have a sharp point.I have tried engraving with such a tool and it didn\'t work too well,so I bought a small range of engraving tools that did come to a sharp point and it helped a lot.The big giveaway was that attempting to engrave a font with serifs had a zone in the serifs that went outside the outline of the lettering;in this case there are no serifs but the absence of a sharply defined line at the bottom of each symbol seems to be a clue.
\r\n \r\n
\r\n
\r\n
I know what your talking about some so called V bits are sharp in the X axis but have a flat in the Y. \r\nThe bit o was using is sharp in both the X and Y directions.. \r\nPhoto attached\r\n
\r\n V carving could be done even with conical ball nose bits, as in attached pictures, but it depends on parameters. \r\nFirst one is with step overs of 60% and 80%, second one with step overs 25% and 80%. \r\nBit used is conical ball nose 16 degrees R0.25mm (0.01").\r\n
\r\n This is from documentation (you should have it on your computer). \r\n \r\nExperiment on some scraps to familiarize yourself with parameters. Also for different materials you can have different step overs (smaller for metal like brass and a bit larger for wood).\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
\r\n It just occurred to me that there are two files involved in my testing for cutting a file 0.020” deep on another file that cuts a section of wood with a 3.00” radius. This is all testing. \r\n \r\nIn the Vcarve V bit file that cuts the character I set flat depth to 0.020” deep, final and clearance pass both to 0.012”, then check Project tool path onto 3D model. \r\n \r\nI just realized because I’ve never V carved on a curved surface before, I must be missing something when cutting on a 3D surface. \r\n \r\nHow does the V Carve know what the surface/radius is when I check Project tool path onto 3D model? \r\n \r\nDo the two files get linked together someway so the the V-Carve knows what the radius it is Projecting to, how do I do that. \r\n \r\nSorry I have been taking a break, I was so frustrated, I went ahead and made the fixture for holding the sword, on the chance I get the cutting operation figured out. \r\n \r\nThanks for sticking with me, this should be a big step forward if I am right in joining the two files together somehow. \r\nHager\r\n
\r\n Hi Hager, \r\nhow V-carve "knows", that\'s are the program\'s internals. \r\n \r\nFind attached an STL and pictures of a simulation on a quite irregular profile. \r\nFinal pass step over: 5% \r\nClearance pass step over: 50% \r\n \r\nAnd another: 60 degrees V bit never reaches 0,2" depth \r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
Hi Hager, \r\nhow V-carve "knows", that\'s are the program\'s internals. \r\n \r\nFind attached an STL and pictures of a simulation on a quite irregular profile. \r\nFinal pass step over: 5% \r\nClearance pass step over: 50% \r\n \r\nAnd another: 60 degrees V bit never reaches 0,2" depth
\r\n \r\n
\r\n
\r\n
So, the program knows whenever I have a 3D model on the screen and place a drawing or TXT file on top of it, and click PROJECT TO SURFACE the drawing or text will automatically be made to conform to the 3D model. Correct? That’s how it knows, and i don’t have to link the two together in VCP some way, correct? \r\n \r\nIf this assumption is correct it answers so many questions I had been struggling with. \r\n \r\nThe photo below are two rectangles 0.040” wide and 1” tall cut on a flat surface. It was drawn over the 3” radius model. The cut on the left was not projected and the one on the right was projected, they look to be the same width in the center and the right one is deeper on the ends, conforming to the radius.\r\n
\r\n What tool was used for those cuts? \nIt does not look as any kind of conical bit \n \nTo better understand V-carving take a look at this video: \n \nhttps://www.youtube.com/watch?v=RY0zLv3wcyc \n \nYou will see some "cross cut" drawings just to make clearer picture. \n \nAnyway, which tool you would like to use (which one do you have) to carve the name of your Chinese friend on the sword grip. I guess that the profile is as per your first post. \nRemember, it has to be a V bit or Conical ball nose.\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
\r\n Thanks Vasto, good information I’ll file it away for when I do any inlays, the fellow that owns the swords is just use black to fill in the cuts on the sword. \r\n \r\nWell the first sword came out perfect on the first cut. But the second sword the new one I hadn’t seen before took three cuts and adjustments to the various parts of the character before it was complete and at correct depth. \r\nThe first sword had one constant sweeping radius that I centered on and it cut perfect at one pass. \r\nNow the second sword profile wasn’t one consistent radius like the first sword but a radius and a down bevel in the area to be cut. And the down bevel wasn’t wide enough to cut the entire character so I had to cut the top character, then edit the top half of the character and cut it deeper so the repair cut matched the depth of the lower half of the character. The bottom character on the radius cut OK. \r\nBoy if I do this again I need some way to define the profile of the area to be cut so VCP knows how deep to cut the variations in the profile. \r\nI added a photo of a red neck parallelogram that I used to rotate the sword in the fixture and set the center of the radius where I wanted the character to be cut, it worked perfect on the sword wher the image area was to be centered on the radius. Not so much on the second sword where Yee image area was spread over a radius and a bevel. \r\nAnyway it’s a done deal. \r\nWould you verify that my thoughts on the 3D model and projected text was correct or not on my previous post \r\nThank you all for your comments and suggestions. \r\nHager\r\n
\r\n Glad to see that you have finished it. \n \nFor any Vcarve/Inlay on irregular surfaces you should have the exact model. \nVectric software do not have a crystal ball to "see" what is on your mind. \nAs any software it does what it is told to do. The more precise input, the outcome will be prettier.\r\n
\r\n
\r\n\r\n \r\n\r\n\r\n
\r\n \r\n \r\n \r\n \r\n
Make no mistake between my personality and my attitude. \r\nMy personality is who I am. My attitude depends on who you are.
This is from documentation (you should have it on your computer).
Experiment on some scraps to familiarize yourself with parameters. Also for different materials you can have different step overs (smaller for metal like brass and a bit larger for wood).
Make no mistake between my personality and my attitude.
My personality is who I am. My attitude depends on who you are.
We use cookies to optimize our website for you and to be able to improve it continuously. By clicking the "Accept" button, you expressly agree to the use of cookies. For further information on cookies, please refer to our privacy policy.
We use cookies to optimize our website for you and to be able to improve it continuously. By clicking the "Accept" button, you expressly agree to the use of cookies. For further information on cookies, please refer to our privacy policy.
\r\n\r\n \r\n 
\r\n \r\n \r\n \r\n 
Reply With Quote
\r\n 
Re: Need STL FILE\r\n 
stock has to be machined to the shape of the model 
Originally Posted by ger21\r\n 
Re: Need STL FILE
