Inlays
The tool diameter offset will be in your CNC control, say for example you use a 10mm tool in fusion and you set it to be 10mm then if you cut a 2D contour then the toolpath which will be the center of the tool will be exactly 5mm from your selection and will cut to the size of your Model/Sketch, all good so far.
Now to make the actual cut of say the 50mm square at the CNC just set the tool diameter in the CNC Control to either a larger/smaller value to move the tool "over", making the value say a diameter of 9.9mm will move the tool "over" by 0.05mm from the line of the toolpath therefore making the part actually 0.1mm smaller so the 50mm square would then be 49.9mm. Hope this made some sort of sense.
The big advantage of using the above method is that you can make very small changes at the CNC Control to get your "fit" without having to keep making changes back in Fusion and generating new code and loading to the machine everytime.
How accurate your parts turn out will depend a lot on just how accurate your CNC Machine is, really needs to be 0.01mm or better for best accuracy, your CNC Manual will tell you what it`s rated at, if it has "Precision Ball Screws" it should be pretty good but if it just has "Lead Screws" then maybe not so good depending on where it was manufactured 🙂 🙂
The scaling should work, it is usually best to have the object in your case the "heart" centered on your "Origin" and use the "Uniform Scale" option.
Can you upload your Fusion f3d file ?? Go to :-
File > Export > Select f3d format > Save to a location on your computer > Then attach it to your reply using the "Attachments" facility below your reply box
Simple Scaling Example shown below and example file attached for you to check, look at the scaled setting, if you play around with that setting you will see the inlay block change size and you can set it to whatever you want 🙂
Apologies for the long winded answer 🙂
Yes, I looked at the tool methods in Linux and no, there does not appear to be any Diameter offset facility, probably one reason it is free, get what you pay for I am afraid, all other softwares for similar use do have that facility !!
So, you will have to as you rightly say have to "lie" to Fusion by setting for example your 0.8 tool to say 0.79 and actually having a 0.8 tool in the machine or a 0.81 and a 0.8 in the machine.
If you use the "Edit Tool" function for one Operation say the Pocket then the tool size will also change in any other Operation in the same program.
What you may be able to do is create multiple tools with the same tool number, I am assuming that you don`t have a tool changer so what you could do is select the appropriate tool for inside/outside, see image below for what you could do.
Just have to be very careful that you always select the right tool for the operation, some better naming in the tool description would probably help, but at least you should be able to "tweak" each one as required 🙂 🙂
John, from what we discovered earlier your LinuxCNC does not have the diameter offset facility so you are not able to control adjustments at the CNC Machine.
So, really the only option you can really use is the "In Computer" side compensation which means that if you use a 10mm End Mill in Fusion and a 10mm End Mill in your CNC then you will get a square the size that you have either Modelled or Sketched, that is assuming that the 10mm EM that you buy is actually 10mm, they are mostly a fraction undersize so you need to some careful measuring for greater accuracy so that whatever the actual tool measures that is the value that you enter in your Fusion Tool Library for your Document so what you cut in Fusion will be cut at the machine assuming accurate machine.
Doesn`t matter what diameter value you put in Linux, the G Code only calls the length offset using a G43 Z** H** number so it just calls that tool number and uses the length offset that you have in Linux for the tool, if you want to physically put a different size tool in the CNC then you can do that and the size of the part cut will be changed, for example you use the "Left side compensation" to follow a shape and program an 8mm diameter tool in Fusion the toolpath generated will be exactly 4mm from whatever you selected and if it is an 8mm tool in Linux and cutting a 20mm square you will get a 20mm square, depending on the actual size of the tool, so, yes, Fusion will cut the correct size 🙂
See the image below for LinuxCNC code, you can see that for the 8mm tool it has a G43 Z20. H8 line, this just calls up that tool that hopefully you have designated as Tool #8 in your LinuxCNC.
Your limitations are at LinuxCNC, not at Fusion, now, as you are unable to make adjustments to the compensation at LinuxCNC you will need to do it in Fusion so some "fudging" will be required and some Math, so, if you are doing a 20mm square and you have an 8mm tool in LinuxCNC then if for example you want to move the toolpath a small amount and make the 20mm say 19.8mm then you need to take an extra 0.1mm off the sides, to do that you can set the tool size in Fusion to 7.9mm, Fusion "seeing" a smaller tool will move it closer to the selected edge so when the code that is generated runs in LinuxCNC with the full size 8mm tool the 20mm square will be cut smaller because the distance from the center of the tool which runs along the toolpath will be greater and so will remove more material.
Hope some of this made some kind of sense 🙂 🙂 🙂
Hey Engineguy,
The offsetting does work in linuxcnc. It's done in the tool table file by changing the diameter of whichever tool is loaded. Afterward reload the tool table and reload the work file for compensation to be applied. I've made quite a few test cuts on the same work file with just simple shapes and can say for sure that adjusting the tool table does alter the tool path. Or should I say the tool's position in relation to the path. I'm just having trouble understanding what the different radius controls in the process setup are doing. I wish I was able make a hundred slightly different pocket processes and look at them at one time.
Anyways, no I've only ever used 'stock to leave' a handful of times. I make sure it's off. Once I can get a better grip on these various settings and adjustments I'll be able to do a roughing pass and finishing pass with the same file and tool or several tools, but all the same code file.
I had acquired a large oak block from a local amish pallet factory and i also have some mahogany on hand. Cut a plank of each on the band saw, faced them on the mill. Ran my 'in control' compensated jobs and here's the result!
The width of the walls that make up the heart face are 2mm. When making this heart project for both the pocket and contour I told fusion that I was using a 0.8mm end mill and fusion continued to give me a hard time about the tool gouging somewhere. I went down to a 0.6mm in fusion and messed around with the radius controls until fusion was happy. I have no idea why it was happy. This is what I'm having trouble understanding.
This was my third attempt with the compensation. I used a 1.2mm end mill in fusion and I believe I used a 0.8 in the spindle while applying the adjustments in the picture below to the linuxcnc tool table. This is 5.25mm plywood. The pocket is 2mm deep, no glue and I can not get these apart.
