2 Attachment(s)
A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
I'm just getting started with practicing with my 1100M, and I have some questions...
I kept getting an error when trying to use the digitizing probe to find my WCS origin, it was something like "probe move would exceed the x axis negative limit". I must be doing something wrong with this probe because I can never get it to work. I did set the length and diamter in the tool table for tool 99 though. Is there a way to use the probe to find X Y and Z zero and tell the pathpilot that's the WCS origin I set in Fusion 360?
I broke an 1/8" endmill on a 2D contour operation, I screenshotted the geometry and tried to attach it to this post, I hope it works. My question is: was the feed rate too fast, and that's why it broke? Or should I have choked up on the endmill more in the collet? The part I was cutting is a scrap piece of box tubing. It broke on the second pass in the bottom left corner of the pocket. I was trying to use a ball endmill to cut a radius around the bottom inside corner.
When I pick a tool in fusion 360 does it have to match my tool in real life in every dimension, or can I just set the tool length in the tool table in path pilot and when it asks for say an 1/8" flat endmill put that tool in?
If I want to engrave lettering what is the best way to do that? Sketch text in Fusion 360 and use trace? The text in Fusion is not made up of thin lines, rather the letters have an area to them. Just pick all the outlines on the top geometry and use negative stock to leave, or pick the outlines at the bottom of however deep I modeled the letters? What is a good endmill to engrave letters in 7075 forged aluminum? (AR lowers)
If I want to cut a 1/8 slot in the surface of a part, can I not use a 1/8 endmill to do that? It seems like Fusion won't create a toolpath for that, so I made the slots a little wider and it did this oscillating thing to cut them, slower but they look alright. Is that just how CNC's work? Why won't it just run the endmill across in a straight line? You can see the thin slots I'm talking about in the sample part below. I want to eventually do milling on Glock slides so I'm trying to practice those types of cuts.
How can I clean up the surface finish of the bottom of this pocket (and the slots)? I used 2D adaptive to create it, can I do a finishing pass in that operation or do I need another operation to finish it, if so what should I use?
Thanks for any and all help!!
Re: A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
If you get an error about exceeding some dimension, then it means that the mill thinks it would have to jog into the limit switches to perform the operation you asked for.
Move your work slightly to give it a little more room. Also, make sure you always "ref axes" for all three axes each time you turn on the mill. If the ref axes indicator isn't green, you're living in a world where the mill is confused about coordinates.
If your 1/8" end mill was a ball nose, then know that the bottom of a ball is much finer than the side, so you typically will want to feed much slower than you'd feed for a square end mill. Use the formula you'd use for plunging, as a first order of approximation (regular feed divided by number of flutes.)
Your picture says nothing about whether you did it right or wrong. What material was it? What was your depth of cut (axial engagement)? What was your radial engagement? How fast did you spin the spindle? How fast was your feed rate? How many flutes, and other cutter shape parameters? Answer those questions and people can give a reasonable estimate of where you might have been off.
When you pick a tool in Fusion, then the diameter of the tool is important, and the height is important if you rely on Fusion to detect collisions with the collet. Assuming you have entered the correct tool height in the offset table, and assuming you set your Z-height correctly, then the mill will put the end of the tool where it "should" be according to Fusion, even if you didn't tell Fusion about the exact height of the tool -- it's referenced by tip-of-tool.
I haven't engraved letters, but I know people use drag engravers for thin and outline type, and vee bits (spinning) for deeper letters. There is some way to make Fusion engrave as deep as it can within the outline of a particular set of letters; I've seen a YouTube tutorial about it somewhere. For good-looking letters, that's what I would do.
If your tool in fusion is exactly-on-the-dot the same width as the slot you've modeled, then Fusion may detect a collision and refuse to generate the toolpath. However, that's generally not a great idea, because the finish of that slot won't be great; you'll want to have some room to cut in the middle, and then run finishing passes (or at least one finishing pass, on the side that you didn't climb cut on.)
The "oscillating thing" is for material removal (Fusion usually calls these "adaptive," and you will want a finish pass at the end of that to clean up the edges. Typically you will want to leave a few thousandth's of an inch of radial "stock to leave" during the slotting operation, so there's something to actually clean up. If you just want to cut along the edges, rather than go sideways in the slot, use a 2D profile toopath, or if the slot is wider than 1.6x your cutter, use a 2D pocketing toolpath (not adaptive.)
Generally, when you want to clean something up, you make some "stock to leave" for radial (sideways) and perhaps axial (bottom) directions. Then you use a finishing pass along the edges, usually with 2D contour or perhaps the pocketing path. Also, some toolpath generators will let you put a checkbox in to generate the finishing pass last. Because the radial engagement is generally quite shallow, you can typically take much deeper cuts (axial engagement) when finishing; you'll want to shave the entire wall in one operation if you can at that point.
Finally, the limiting factors for spindle speed (RPM) are your cutter materials/coatings compared to the material you're cutting (surface speed,) and the spindle horsepower if you have bigger cutters/deeper cuts. If you think you're taking too much feed rate, you can take less per tooth by increasing the RPM while keeping feed rate constant (assuming you're not at the limit of your spindle.) Meanwhile, if you get a lot of chatter, you can try reducing RPM and perhaps increasing feed a little bit, which generally will quiet down chatter, although at some point that will overload the bit and break it.
Re: A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
With respect to engraving text, selecting Trace or Engrave in Fusion depends on what text format you are using. The "space between the lines" that you refer to is because you are using TrueType fonts, which are, essentially, a vector graphic - ie. the text is defined by a geometry around an invisible centerline, it is not a graphic. So, Fusion will put the tool path on the outside lines and trace or engrave that because that is how the geometry is defined. Both trace and engrave will do that to TrueType text. If you want just a single line (instead of the double line text you'll otherwise get), you need to obtain special single-line fonts or software that will convert your fonts to single-line fonts.
Now, if your text is not an actual font, but rather a graphic (like a logo for example), then trace and engrave will behave differently. If you simply lay that graphic down on the surface of your part, then both trace and engrave will again do the same thing (assuming you've set the engrave tool to go below the surface). However, if you impress the text to some depth, then they will behave differently. The trace function will again simply trace the contour. But the engrave function will travel the centerline and will vary it's depth in order to keep the width exactly between and up to the lines.
I suspect you're using fonts - in which case your best bet is to get single line fonts.
Re: A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
Quote:
Originally Posted by
jwatte
If you get an error about exceeding some dimension, then it means that the mill thinks it would have to jog into the limit switches to perform the operation you asked for.
Move your work slightly to give it a little more room. Also, make sure you always "ref axes" for all three axes each time you turn on the mill. If the ref axes indicator isn't green, you're living in a world where the mill is confused about coordinates.
If your 1/8" end mill was a ball nose, then know that the bottom of a ball is much finer than the side, so you typically will want to feed much slower than you'd feed for a square end mill. Use the formula you'd use for plunging, as a first order of approximation (regular feed divided by number of flutes.)
Your picture says nothing about whether you did it right or wrong. What material was it? What was your depth of cut (axial engagement)? What was your radial engagement? How fast did you spin the spindle? How fast was your feed rate? How many flutes, and other cutter shape parameters? Answer those questions and people can give a reasonable estimate of where you might have been off.
When you pick a tool in Fusion, then the diameter of the tool is important, and the height is important if you rely on Fusion to detect collisions with the collet. Assuming you have entered the correct tool height in the offset table, and assuming you set your Z-height correctly, then the mill will put the end of the tool where it "should" be according to Fusion, even if you didn't tell Fusion about the exact height of the tool -- it's referenced by tip-of-tool.
I haven't engraved letters, but I know people use drag engravers for thin and outline type, and vee bits (spinning) for deeper letters. There is some way to make Fusion engrave as deep as it can within the outline of a particular set of letters; I've seen a YouTube tutorial about it somewhere. For good-looking letters, that's what I would do.
If your tool in fusion is exactly-on-the-dot the same width as the slot you've modeled, then Fusion may detect a collision and refuse to generate the toolpath. However, that's generally not a great idea, because the finish of that slot won't be great; you'll want to have some room to cut in the middle, and then run finishing passes (or at least one finishing pass, on the side that you didn't climb cut on.)
The "oscillating thing" is for material removal (Fusion usually calls these "adaptive," and you will want a finish pass at the end of that to clean up the edges. Typically you will want to leave a few thousandth's of an inch of radial "stock to leave" during the slotting operation, so there's something to actually clean up. If you just want to cut along the edges, rather than go sideways in the slot, use a 2D profile toopath, or if the slot is wider than 1.6x your cutter, use a 2D pocketing toolpath (not adaptive.)
Generally, when you want to clean something up, you make some "stock to leave" for radial (sideways) and perhaps axial (bottom) directions. Then you use a finishing pass along the edges, usually with 2D contour or perhaps the pocketing path. Also, some toolpath generators will let you put a checkbox in to generate the finishing pass last. Because the radial engagement is generally quite shallow, you can typically take much deeper cuts (axial engagement) when finishing; you'll want to shave the entire wall in one operation if you can at that point.
Finally, the limiting factors for spindle speed (RPM) are your cutter materials/coatings compared to the material you're cutting (surface speed,) and the spindle horsepower if you have bigger cutters/deeper cuts. If you think you're taking too much feed rate, you can take less per tooth by increasing the RPM while keeping feed rate constant (assuming you're not at the limit of your spindle.) Meanwhile, if you get a lot of chatter, you can try reducing RPM and perhaps increasing feed a little bit, which generally will quiet down chatter, although at some point that will overload the bit and break it.
Awesome, I actually got an email response from Tormach on the probe thing and you're both right. I set the zero in the "center" of the table travel and ran the probe routine again and it worked fine. Thanks for the note about referencing the axes, I didn't know that. On a related note, how do I get the path pilot to keep my tool lengths when I turn the machine off? It keeps erasing them and I have to set the probe up every time I turn the machine on.
As far as my broken endmill, I was cutting .050" into box tubing (scrap I found in my barn). I screen shotted the speeds/feeds it must not be showing up. Spindle was 6500, .002 feed per tooth, surface speed was 212.7 ft/min, feed rate was 26 in/min. It was a 2 flute 1/8" ball endmill TiAIN coated. I used a square end mill to cut the pocket, then I used 2D contour to radius the inside bottom corner of the pocket, so I chose the bottom inside line in the model so the ball end mill would just follow it and create the radius. For some reason it's going deeper than I thought, I think I need to add some axial stock to leave because I tried this again at a much lower feed rate in aluminum, and although it didn't break the endmill the cut is too deep around the bottom, it's like it's sinking the middle of the "ball" to that depth rather than just touching the surface. I guess that makes sense.
I saw that engraving tutorial too, but I couldn't really replicate what he did. It was a video on trace vs engrave.
Thanks for the tips on finishing passes, do smaller diameter cutters create more tool marks than larger ones?
How do you control the radial engagement in Fusion 360? I seem to be able to adjust feed per tooth, feedrate, stock to leave, depth of multiple cuts etc pretty well, but I can't figure out how to control radial engagement or how big of a "bite" I'm taking.
- - - Updated - - -
Quote:
Originally Posted by
dannirr
With respect to engraving text, selecting Trace or Engrave in Fusion depends on what text format you are using. The "space between the lines" that you refer to is because you are using TrueType fonts, which are, essentially, a vector graphic - ie. the text is defined by a geometry around an invisible centerline, it is not a graphic. So, Fusion will put the tool path on the outside lines and trace or engrave that because that is how the geometry is defined. Both trace and engrave will do that to TrueType text. If you want just a single line (instead of the double line text you'll otherwise get), you need to obtain special single-line fonts or software that will convert your fonts to single-line fonts.
Now, if your text is not an actual font, but rather a graphic (like a logo for example), then trace and engrave will behave differently. If you simply lay that graphic down on the surface of your part, then both trace and engrave will again do the same thing (assuming you've set the engrave tool to go below the surface). However, if you impress the text to some depth, then they will behave differently. The trace function will again simply trace the contour. But the engrave function will travel the centerline and will vary it's depth in order to keep the width exactly between and up to the lines.
I suspect you're using fonts - in which case your best bet is to get single line fonts.
How do I find single line fonts for Fusion 360?
Re: A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
Quote:
how do I get the path pilot to keep my tool lengths when I turn the machine off? It keeps erasing them and I have to set the probe up every time I turn the machine on
That seems wrong. If you enter a value into the "Offsets" tab table, it should preserve the values across restarts. It's stored in a tooltable file named ... I think mill_data/tool.tbl in the home directory of the "Operator" user.
If you're not a Linux person, you might be able to call Tormach to troubleshoot it with them.
Quote:
How do you control the radial engagement in Fusion 360?
If you're using a Contour toopath, you cannot. For various pocketing/clearing toolpaths, there are typically "stepover" or "maximum engagement" parameters on the tool path tab that end up controlling how much sideways it will cut.
Note that slots or initial cuts/ramps will likely always have 100% engagement if you don't pre-drill with a big drill and use that as your plunge/ramp area. Hence, you may wish to adjust feeds/speeds for ramping or plunging.
0.002 per tooth for an 1/8" ball nose sounds very aggressive, even if you're cutting in aluminum. In fact, it's a little bit aggressive even for a 1/8" square nose, but for carbide in softer materials it should do fine.
Regarding tool marks: think of it as the tool taking successive nibbles out of the wall using a circle that slides along the wall. The shallower the bite is, and the larger the tool diameter is, the "flatter" those nibbles will be, and the better the finish.
(There are additional metallurgical phenomena related to the material bending minutely, which I couldn't begin to explain. Those matter once you want to push to the limit.)
A larger tool will always leave a better surface finish when using the same feed per tooth and radial depth of cut, because the angle of "nibbling" will be shallower. Or, for a given surface speed and finish, you can feed faster with a bigger tool -- same relation.
Re: A TON of Questions (Probe, Engraving, WCS, Broken Endmill)
Quote:
Originally Posted by
The_Wound_Channel
How do you control the radial engagement in Fusion 360?
You control it in different ways depending on the tool path you've selected:
2D Contour - Passes tab, controlled with "Roughing Passes" as well as "Multiple Finishing Passes" + "Stepover"
2D & 3D Adaptive - Passes tab, "Optimal Load" setting
Others are similar. Check the passes tab and fiddle with the settings.
Always, always run a simulation with the stock sized accurately and check for gouges or crashes.
Fusion has some single-line fonts built in now. In addition, you can download stick fonts off the internet. Once you've installed the fonts in your computer (Windows), the next time you start F360 they will be available.
