How to enter tapered ball nose bits into Vectric tool database
How to enter the correct settings for tapered ball nose bits into the Vectric tool database. These bits work perfect for cutting 3D designs. This lesson applies to Vectric VCarve, Aspire, and Cut2D.
Want to learn more??
Click the link below to take your Vectric skills to the next level!
Video Transcript:
Hello everyone. In this lesson we're gonna learn how to enter tapered ball nose bits into Vectric's tool database. So these bits are generally used for 3D projects, and you could see at the base of the bit, it would generally be around a quarter inch in diameter, and then it usually tapers down to a smaller point.
So that gives you the strength of that quarter inch shank, but the detail of these smaller tips. And this is the exact set that I use, I will link it down below in the description if you wanna check it out. But this one is from ToolsToday, and these are Amana bits. So down here we're gonna look at our settings.
We need to know the sizes of all these bits. And this particular one is a set. So we're gonna look at one individual bit. So let's go with that smallest one there, and that will be this one here with the one 64th inch radius tip. So we're gonna click view details on that particular one. And you can see now it's isolating just that bit.
And if you scroll down, this is on Toolstoday's website, every website's gonna be a little bit different depending on where you're getting these bits from. But you should have all the measurements available from the manufacturer. So if you go to this diagram right here, We could see the diameter of the shank, the length of the bit, the length of the cutting flutes, the angle of the bit, the radius of the very tip and the diameter of the tip.
So we don't actually need all of those measurements, but some of those we are definitely going to need to enter it into Vectric software. And I will give you a heads up uh, a lot of people use the downloadable files that you can import right into Vectric. That is great, but only if they're correct. A lot of these, especially from toolstoday, I've found that the information was not actually entered correctly into these files for the tapered ball nose bits, and a lot of people have been messing up their projects because they have the wrong information.
So personally I like to enter the tool myself into the tool database. That way I know all the information should be correct or you could download it and then just double check all the information and change anything that's needed. Okay, so let's jump into Vectric software, this can be done in Cut2d, VCarve, or Aspire.
And we want to open up our tool database. So we can either do that inside of any of the toolpaths, or we can click this button here that says display tool database. Or finally, you can also go up to the toolpath at the top and click tool database at the bottom there. That will open up your tool database.
And first we need to select where we want to place these tapered ball nose. So by default, you should have a section that says Ball nose, so you can click on that group and when you add a new tool, it'll automatically go in that group. Or you can add in a new group by selecting the very top group, which would be the imperial tools.
And of course you can also do metric if you wanted to do metric. And you could see I made my own group down here that says 3D Tools, and I entered all my tapered ball noses in there. So to do that, you could select the imperial tools down here at the bottom, you want to click add a group. And then in here where the name is, we would name that.
So we can even say TBN for tapered ball nose. You can add some notes if you like, and then click apply. Okay, so now we have a new group created. So we wanna select that group and then at the very bottom, click this little plus sign and that will add a new tool into that group. And like I said, you don't have to make that new group, you can also put it in the ball nose section if you wanted to.
But in this group now we have a new tool started. So for tool type, you want to drop this box down and you wanna select tapered ball nose, select that, and that will change some settings to be applied for tapered ball nose. So this is the part where a lot of people get confused on what numbers to place in here.
So we're gonna go back to the ToolsToday website, and we need the information from this particular bit. So the first thing Vectric was asking for was the diameter. And this diameter is the diameter of the shank, where the top of this bit is, not the diameter of the bottom. So that would be this lowercase letter D, which is down here in this chart, and that is one quarter of an inch.
So back in Vectric software where it says diameter, that will be a quarter inch, which is our shank diameter. So it's correct right now, and units we are in inches. But of course you can also do this in metric. Next we have side angle, and you could see the chart on the side here that is the angle from the center of the bit to the edge of the tapered ball nose.
So if you go back to our chart, you could see right here is the lowercase letter A for the angle, and that is reading the same angle from the edge to the center of the bit. So that is right here, 6.2 degrees. So back in Vectric software, where it says side angle, we are going to enter 6.2 degrees. Next we need tip radius.
And this is the part that's usually messed up on the imported files that ToolsToday has created. So if somebody may have gotten mistaken, they put the wrong radius and that will mess up how your tool carves, so you wanna make sure this number is correct. So if we go back to our chart, that will be this uppercase letter R.
So that's right here, 1/64th. A lot of people accidentally use the diameter instead of the radius, so you wanna make sure you're using the radius. So that's 1/64th for this bit. So for the radius, if you know the exact decimal place of 1/64th, you can type that in there, but most likely you're not gonna know that.
So you could type in number 1/64. So that is 1/64th, and then click the equal sign and then that will automatically get you the decimal number of that fraction. And then finally, we need to know the number of flutes. This is optional, this is more for getting your feed and speed settings.
But if we go back to our chart, you could see this particular bit has three flutes. So in vectric software, we are going to enter three there. And that's all the geometry settings we need. So now we would click create settings and now that will give us more cutting parameters and the feed and speeds. So I'm just gonna give you some general numbers to work with here.
Of course, you're gonna change this depending on your machine, but for the pass depth, this is a very tiny bit on the very tip of it. So you don't wanna go too deep with this, but most of the time you're actually not cutting that much material. And if you use the 3D finishing toolpath, which is what this tool is usually used for, it goes a full depth pass anyways.
And it will ignore this pass depth number, so keep that in mind as well. But generally speaking, around one eighth should be okay for this because it does taper, so it does have some more strength. But that's where I'll start out with. You can always change that depending on what you're doing and what materials you're working with.
For a stepover if you want a very nice finish, I generally go around 8% for the percentage. That will give you a very nice finish, but it will also take a little bit more time to machine, but you're also gonna save a lot of sanding time. So I generally like to let the machine do all of the work where I don't have to sand as much at the end.
If you wanna machine it a little bit faster, you can bump this up to 10%, but you may not save that much time and you may get less quality finish, so I generally go around 8%. Clearance pass, stepover you're most likely not gonna use that this much with this particular tool because you're gonna be using it for the finishing.
But generally speaking, I would do it around 20%, you can just leave it right there. But like I said, you're most likely not gonna use that too much. All right, now we're gonna come down here for the feed and speed settings. So I generally like to go off of what the tool manufacturer recommends and then I adjust from there as needed.
So for ToolsToday's website, you have to go to download and then you'll see a CNC feed and speed chart, click download and that will be the pdf. So with this particular tool, it is the three flute ball nose, and the flutes are gonna matter for the feed and speeds. Generally speaking, more flutes allow you to go a little bit faster.
We can also double check the tool number over here. So let's zoom into this a little bit so we can see what we're working with. And this particular tool is going to be the diameter here of the tip 1/32nd. So that's what's gonna be in this chart here, 1/32nd inch diameter for the tip, and the tool number we could see is 46280-K.
So in this chart, we can double check to make sure we have that same number there, which we do. So that means this is the correct chart. So now down here we have some different settings, depending on the material you're using. Most of us are using wood, so we would go off of this particular row. But if you're cutting plastics, acrylics, or plexiglass, then you're gonna use these settings up at the top.
So here you could see for wood, MDF and sign- foam, they recommend between 40 and 100 inches per minute. And that will give you a chip load of these figures right here. And that's based on 18,000 RPMs. So back in our settings, the RPMs right here at the top is gonna be 18,000. We're gonna go with inches per minute.
And the feed rate, if we go back to that chart, is between 40 and 108. So depending on your machine is gonna depend on where you go with this. If you're just starting out, I would start out the lower figure and work your way up. If you're very comfortable with your machine, you could start out at the higher figure, or you can just go somewhere in the middle.
So I generally go a little bit in the middle to the high end for my particular machine, but I am more comfortable with that. But you may not be so you can start out slower, but just keep in mind it will take a lot of extra time to machine at these slower rates. And generally you're not cutting that much material with the tapered ball nose, so you can get away with higher speeds.
So for this example, I will go somewhere in the middle, let's say around 80 inches per minute. So that will be for the feed rate. So the plunge rate is generally half of that. So if we go back to Vectric, let's say we make the feed rate 80 interest per minute. So the plunge rate is generally half of that, which would be 40.
Okay, and tool number only applies if you're using an automatic tool changer. All right, so that should be all you need to enter. You wanna double check this chip load number, and this chip load is calculated by the number of flutes, the feed rate, and this spindle speed. So those are the only three numbers that change this chip load.
So by the three numbers we entered there, that gives us a chip load of 0.0015. So we wanna go back to this chart and make sure you're within this range here. Which in this case we are, so that's gonna optimize your chip load for this particular tool. And if you look at Amana's charts here too, they also recommend the depth of cut to be one times a diameter.
And that's for these feeds up here. If you go two times a diameter for the depth of cut, they recommend reducing the feed rate by 25%, and then three times they recommend reducing by 50%. These are just general recommendations, but that's something you can look out for as well. Depending how deep you're cutting.
So in our chart, by going by that logic, the diameter of the tool will be 1/32nd. So they would actually recommend 1/32nd for this pass depth. So you could type in 1/32 equals, and that right there is what they would recommend for the pass depth. But like I said, when you're using tapered ball noses, this is generally ignored anyways when you're using the 3D finished toolpath.
Okay, so we're just gonna click apply to save all those changes, so that just saved that tool in that group. And keep in mind too, we also were in hardwood and we had our machine selected, so it'll save for those two as well. So you can also add in more materials or more machines to save different settings for each one.
But we can also enter in any notes you have about the tool and you can change the name if you like. One thing I like to do is change the tip on the name to be the diameter and not the radius. That way it's easier for me just to visualize what tip we are using. So right here I click edit, and that will be right here where it says tip.
And then it has this tip radius. So we're gonna erase that radius. And that was a variable and can enter variables by right clicking and finding them here. And that was the tip radius down here. Unfortunately they don't have a tip diameter, so we have to manually type that in. And I also like to make that a fraction so it's easier to recognize.
So for this particular tool, it is 1/32nd inch for the tip diameter, so that's what I'm gonna enter in there. We can also enter in the tool number and here as well if you wanted to. But in this case, I'm just gonna leave it as is. I also like to deselect this so it doesn't set that as a default. Otherwise it's gonna change that for every new tapered ball nose you enter.
Okay, so now we're gonna click okay. That changed the name, and now we're all good to go. So now when you see this, it will say, tip 1/32nd, and you know exactly what tool you're working with. Okay, so that's how you enter in a tapered ball nose into Vectric software. And those same steps will apply for any size tapered ball, nose bit you may enter.
And as always, if you have any questions, just let me know.
So that gives you the strength of that quarter inch shank, but the detail of these smaller tips. And this is the exact set that I use, I will link it down below in the description if you wanna check it out. But this one is from ToolsToday, and these are Amana bits. So down here we're gonna look at our settings.
We need to know the sizes of all these bits. And this particular one is a set. So we're gonna look at one individual bit. So let's go with that smallest one there, and that will be this one here with the one 64th inch radius tip. So we're gonna click view details on that particular one. And you can see now it's isolating just that bit.
And if you scroll down, this is on Toolstoday's website, every website's gonna be a little bit different depending on where you're getting these bits from. But you should have all the measurements available from the manufacturer. So if you go to this diagram right here, We could see the diameter of the shank, the length of the bit, the length of the cutting flutes, the angle of the bit, the radius of the very tip and the diameter of the tip.
So we don't actually need all of those measurements, but some of those we are definitely going to need to enter it into Vectric software. And I will give you a heads up uh, a lot of people use the downloadable files that you can import right into Vectric. That is great, but only if they're correct. A lot of these, especially from toolstoday, I've found that the information was not actually entered correctly into these files for the tapered ball nose bits, and a lot of people have been messing up their projects because they have the wrong information.
So personally I like to enter the tool myself into the tool database. That way I know all the information should be correct or you could download it and then just double check all the information and change anything that's needed. Okay, so let's jump into Vectric software, this can be done in Cut2d, VCarve, or Aspire.
And we want to open up our tool database. So we can either do that inside of any of the toolpaths, or we can click this button here that says display tool database. Or finally, you can also go up to the toolpath at the top and click tool database at the bottom there. That will open up your tool database.
And first we need to select where we want to place these tapered ball nose. So by default, you should have a section that says Ball nose, so you can click on that group and when you add a new tool, it'll automatically go in that group. Or you can add in a new group by selecting the very top group, which would be the imperial tools.
And of course you can also do metric if you wanted to do metric. And you could see I made my own group down here that says 3D Tools, and I entered all my tapered ball noses in there. So to do that, you could select the imperial tools down here at the bottom, you want to click add a group. And then in here where the name is, we would name that.
So we can even say TBN for tapered ball nose. You can add some notes if you like, and then click apply. Okay, so now we have a new group created. So we wanna select that group and then at the very bottom, click this little plus sign and that will add a new tool into that group. And like I said, you don't have to make that new group, you can also put it in the ball nose section if you wanted to.
But in this group now we have a new tool started. So for tool type, you want to drop this box down and you wanna select tapered ball nose, select that, and that will change some settings to be applied for tapered ball nose. So this is the part where a lot of people get confused on what numbers to place in here.
So we're gonna go back to the ToolsToday website, and we need the information from this particular bit. So the first thing Vectric was asking for was the diameter. And this diameter is the diameter of the shank, where the top of this bit is, not the diameter of the bottom. So that would be this lowercase letter D, which is down here in this chart, and that is one quarter of an inch.
So back in Vectric software where it says diameter, that will be a quarter inch, which is our shank diameter. So it's correct right now, and units we are in inches. But of course you can also do this in metric. Next we have side angle, and you could see the chart on the side here that is the angle from the center of the bit to the edge of the tapered ball nose.
So if you go back to our chart, you could see right here is the lowercase letter A for the angle, and that is reading the same angle from the edge to the center of the bit. So that is right here, 6.2 degrees. So back in Vectric software, where it says side angle, we are going to enter 6.2 degrees. Next we need tip radius.
And this is the part that's usually messed up on the imported files that ToolsToday has created. So if somebody may have gotten mistaken, they put the wrong radius and that will mess up how your tool carves, so you wanna make sure this number is correct. So if we go back to our chart, that will be this uppercase letter R.
So that's right here, 1/64th. A lot of people accidentally use the diameter instead of the radius, so you wanna make sure you're using the radius. So that's 1/64th for this bit. So for the radius, if you know the exact decimal place of 1/64th, you can type that in there, but most likely you're not gonna know that.
So you could type in number 1/64. So that is 1/64th, and then click the equal sign and then that will automatically get you the decimal number of that fraction. And then finally, we need to know the number of flutes. This is optional, this is more for getting your feed and speed settings.
But if we go back to our chart, you could see this particular bit has three flutes. So in vectric software, we are going to enter three there. And that's all the geometry settings we need. So now we would click create settings and now that will give us more cutting parameters and the feed and speeds. So I'm just gonna give you some general numbers to work with here.
Of course, you're gonna change this depending on your machine, but for the pass depth, this is a very tiny bit on the very tip of it. So you don't wanna go too deep with this, but most of the time you're actually not cutting that much material. And if you use the 3D finishing toolpath, which is what this tool is usually used for, it goes a full depth pass anyways.
And it will ignore this pass depth number, so keep that in mind as well. But generally speaking, around one eighth should be okay for this because it does taper, so it does have some more strength. But that's where I'll start out with. You can always change that depending on what you're doing and what materials you're working with.
For a stepover if you want a very nice finish, I generally go around 8% for the percentage. That will give you a very nice finish, but it will also take a little bit more time to machine, but you're also gonna save a lot of sanding time. So I generally like to let the machine do all of the work where I don't have to sand as much at the end.
If you wanna machine it a little bit faster, you can bump this up to 10%, but you may not save that much time and you may get less quality finish, so I generally go around 8%. Clearance pass, stepover you're most likely not gonna use that this much with this particular tool because you're gonna be using it for the finishing.
But generally speaking, I would do it around 20%, you can just leave it right there. But like I said, you're most likely not gonna use that too much. All right, now we're gonna come down here for the feed and speed settings. So I generally like to go off of what the tool manufacturer recommends and then I adjust from there as needed.
So for ToolsToday's website, you have to go to download and then you'll see a CNC feed and speed chart, click download and that will be the pdf. So with this particular tool, it is the three flute ball nose, and the flutes are gonna matter for the feed and speeds. Generally speaking, more flutes allow you to go a little bit faster.
We can also double check the tool number over here. So let's zoom into this a little bit so we can see what we're working with. And this particular tool is going to be the diameter here of the tip 1/32nd. So that's what's gonna be in this chart here, 1/32nd inch diameter for the tip, and the tool number we could see is 46280-K.
So in this chart, we can double check to make sure we have that same number there, which we do. So that means this is the correct chart. So now down here we have some different settings, depending on the material you're using. Most of us are using wood, so we would go off of this particular row. But if you're cutting plastics, acrylics, or plexiglass, then you're gonna use these settings up at the top.
So here you could see for wood, MDF and sign- foam, they recommend between 40 and 100 inches per minute. And that will give you a chip load of these figures right here. And that's based on 18,000 RPMs. So back in our settings, the RPMs right here at the top is gonna be 18,000. We're gonna go with inches per minute.
And the feed rate, if we go back to that chart, is between 40 and 108. So depending on your machine is gonna depend on where you go with this. If you're just starting out, I would start out the lower figure and work your way up. If you're very comfortable with your machine, you could start out at the higher figure, or you can just go somewhere in the middle.
So I generally go a little bit in the middle to the high end for my particular machine, but I am more comfortable with that. But you may not be so you can start out slower, but just keep in mind it will take a lot of extra time to machine at these slower rates. And generally you're not cutting that much material with the tapered ball nose, so you can get away with higher speeds.
So for this example, I will go somewhere in the middle, let's say around 80 inches per minute. So that will be for the feed rate. So the plunge rate is generally half of that. So if we go back to Vectric, let's say we make the feed rate 80 interest per minute. So the plunge rate is generally half of that, which would be 40.
Okay, and tool number only applies if you're using an automatic tool changer. All right, so that should be all you need to enter. You wanna double check this chip load number, and this chip load is calculated by the number of flutes, the feed rate, and this spindle speed. So those are the only three numbers that change this chip load.
So by the three numbers we entered there, that gives us a chip load of 0.0015. So we wanna go back to this chart and make sure you're within this range here. Which in this case we are, so that's gonna optimize your chip load for this particular tool. And if you look at Amana's charts here too, they also recommend the depth of cut to be one times a diameter.
And that's for these feeds up here. If you go two times a diameter for the depth of cut, they recommend reducing the feed rate by 25%, and then three times they recommend reducing by 50%. These are just general recommendations, but that's something you can look out for as well. Depending how deep you're cutting.
So in our chart, by going by that logic, the diameter of the tool will be 1/32nd. So they would actually recommend 1/32nd for this pass depth. So you could type in 1/32 equals, and that right there is what they would recommend for the pass depth. But like I said, when you're using tapered ball noses, this is generally ignored anyways when you're using the 3D finished toolpath.
Okay, so we're just gonna click apply to save all those changes, so that just saved that tool in that group. And keep in mind too, we also were in hardwood and we had our machine selected, so it'll save for those two as well. So you can also add in more materials or more machines to save different settings for each one.
But we can also enter in any notes you have about the tool and you can change the name if you like. One thing I like to do is change the tip on the name to be the diameter and not the radius. That way it's easier for me just to visualize what tip we are using. So right here I click edit, and that will be right here where it says tip.
And then it has this tip radius. So we're gonna erase that radius. And that was a variable and can enter variables by right clicking and finding them here. And that was the tip radius down here. Unfortunately they don't have a tip diameter, so we have to manually type that in. And I also like to make that a fraction so it's easier to recognize.
So for this particular tool, it is 1/32nd inch for the tip diameter, so that's what I'm gonna enter in there. We can also enter in the tool number and here as well if you wanted to. But in this case, I'm just gonna leave it as is. I also like to deselect this so it doesn't set that as a default. Otherwise it's gonna change that for every new tapered ball nose you enter.
Okay, so now we're gonna click okay. That changed the name, and now we're all good to go. So now when you see this, it will say, tip 1/32nd, and you know exactly what tool you're working with. Okay, so that's how you enter in a tapered ball nose into Vectric software. And those same steps will apply for any size tapered ball, nose bit you may enter.
And as always, if you have any questions, just let me know.
