Obviously the cuts are wider than designed, so the structures are not acceptable.
Thought get a new one, this time with 15 deg sharp tip, was delivered with a really decent tip, cut my finger a little.
Now the tip very soon became dull: it is my impression that already Z-zeroing broadened the very sensitive tip, also IMO the bit setting process dulled it further, and the very first cuts also made the tip much less accentuated, and it is no surprise that the result is not much different. Of course, because when the cutter cuts into the material into a depth that expects a very sharp tip but it is not as sharp the cut path is wider on the surface.
Now there are V-carve bits with a defined tip diameter. I could not find in CC how to tell the database the diameter of the tip, I think CC always assumes a 0-tip.
A 1/32 bit would not carve the details as pocket.
I have seen coin size cuts, so there might be a way to cut very fine structures.
Take a close look at the tip of your 20 degree vee bit. Some vee bits have a rounded tip and others get the tip broken off since they are quite delicate. CC expects a sharp point on the end of your vee bit. If your tip does not go to a sharp point then the carving will not be the correct depths because the vee bit cuts deeper than what you expect. You might need to get a magnifier glass out to inspect the tip of the vee bit.
I will preface this by saying that the smallest emblem I have cut in brass was about 1x2 inches with a 32nd in endmill. So, for what its worth: looking at the size of the details in the iron, there are letters which are 0.0044 inch (~1/256in) apart. Even if the iron could be cut with a 15 degree v bit, the depth of cut between letters this near to each other would only be ~0.015 inch (~1/64 in) deep . I question if that would be deep enough for a functional branding iron.
You are right, I don’t have any idea whether this will make a nice iron at the end! it is a try certainly! Never branded something! Still lasering the product is an alternative! We will see… Since as my wife says I am sometimes a little stubborn (she indeed did not use the words “simetimes” and “a little”) I need to make the piece first and see then.
Guy: I usually use a microscope for that purpose, but don’t need this here: the tip of the 15deg bit is certainly broken off or worn to the unarmed eye. The bit I got was described as usable for aluminum, not for brass. Will try another one, as William said possibly the one I got was not specified for Brass.
The 502 has an included angle of 40 degrees which will reduce the depth of the engraving significantly. Geometrically this is far worse than the 15 degree v bit for this cut. It will be useless as a branding iron (but a good exercise in milling), unless you are willing to go up in size. Success can be approached with a 1/32 inch end mill by increasing the overall iron size (110-120%??), changing the font to a larger one with a much narrower stroke width, and reducing the size of the graphic logo. Essentially, anything you want burned can be narrowed as the contrast will make it visible more than its size. By narrowing these elements you gain distance between them with a goal of 1/32 inch, allowing pocketing with a 1/32 inch end mill. DOC of around 0.100 inch should prevent scorching (according to AI). If you can pick a font/size that allows detail with “G”, “A”, “W”, and “X” , with a 1/32 end mill, you are there. Cheers.
Bozo, thanks!!! Your lesson steeped my learning curve! So essentially a V-carve is not the best idea for a branding iron, it must be a straight bit: understood!
And the pattern must be adjusted that the details may be carved with such a bit. Got it! And rather fine details than wide ones. Will give it a shot! Thanks a lot!
Branding irons with less detail might be cut with a v bit / vcarve tool path. Due to lack of experience with v bits in metal, I would avoid it but others here may do it. I suspect it would require very shallow depths of cut and going through multiple bits might be unavoidable.
I spent a few hours with your design and modified it with the intent of only using a 1/32 inch flat end mill. This is only because I know cutting brass with a 1/32 to the depth needed for an iron is not that difficult. In your design, I ran into issues with the G, A, W, and X because the 1/32 inch bit did not give acceptable detail for the font/size in the design. I had to make a lot of modifications and was not happy with the look. Here is an SVG just to show how much detail had to be removed. I did not pursue enlarging the iron.
Narrowing the text strokes as much as I did also may not be wise for a branding iron because those thin letters may lose heat too fast. By the time the iron gets to the wood, the thin lines may be too cold to burn. Until yesterday, I did not realize the scope of design requirements for a branding iron. There is more than meets the eye. Cheers.
Thank you very, very much for the input. Learned a lot from your post:It is not just sufficient to transfer an object to a g code, it’s also necessary to adjust an object that it can be carved properly, Especially for branding irons. I’m completing new on the field of branding irons and carving brass, so your help steepened my learning curve!
Just putting this out there: PixelCNC allows for tapered endmills with a flat on the tip, but you’ll have to define them with the taper angle (i.e. half of the V-bit angle) whereas with a proper V-bit you just put the angle of the V in the tool definition.
Then the tool can be used to generate a V-carving cutpath, at least wherever the contour being used isn’t narrower than the specified tip diameter for the cutting tool definition being used.
