Hello CAD specialists and machinists. To start off, I am neither.
Here is what we are trying to do, what we are using, and the results we are getting.
Inventor Pro 2016 STUDENT ADDITION, Inventor HSM EXPRESS, Tormach PCNC (770). We are doing some simple testing to make sure we understand the basics of using this system.
A simple part is built in Inventor that includes a .06125 deep oval pocket. A couple inches away from it is a 1.125 inch diameter through hole, for mounting a bearing. We are using scrap pieces of 1"X2" .125" wall 6061 aluminum tube as our test material. We are using a .5" dia., 2 flute, HSS end mill to do the work. We are running approx 1700 RMP, and .0011 IPT, so we are not stressing the system much at all.
The pocket turns out as expected. The problem is, the hole ends up being 1.085" in diameter. They are round and the walls are not tapered. (We saw similar results last year when doing similar work on our “Fireball” desktop CNC routers, but that is another story.)
What would account for the .040" undersized hole?
I know there will be many questions, but this is what I can think of for now.
That number, .040", is way to suspicious. I know that for Fusion360, the default “stock to leave” is the same .020". You can either make it leave no extra stock, or do a second “finishing” operation to clear out the remaining stock.
.020 is the default stock to leave for HSMExpress, and I have found that this often gets put on for default for pockets (and pretty much always for adaptive clearing). What machining technique are you using for this? As a heads up, if you are using adaptive clearing, you want to make sure to use a contour feature to get a smooth contour. If it is a pocket feature, you can use the add finish pass option to get a finish pass. A finish pass is recommended if you are looking to get a bearing fit.
I would recommend leaving it disabled. I will sometimes use it to compensate for bore size. For instance, if the model is 1.125 and we want a 1.124 hole without changing the model, we will put stock to leave as .0005 (leaving stock to leave for Z at 0). You can also leave negative stock to oversize something (ie -.0005 to get a 1.126 hole).
To get a good bearing size, I would recommend turning on a finish pass of about .005. This reduces cutter deflection and gives you a better finish and a more consistent size.
Also, you need to figure out what size your endmill actually is. Endmills are generally toleranced under (like +.000, -.002). Best way to figure this out is do a test cut, measure the part, and then take the difference as the difference in endmill size. It is hard to measure an internal bore well, so I would recommend calibrating your cutter on an external size (using micrometers would help). You can either change the endmill size in HSMExpress and re-post the code, or turn on cutter compensation for the critical features and then enter the size offset in the tool table on the machine. I do not know how tormach handles this, but it is pretty straight forward on a HAAS. Trick is making sure you get the cutter compensation in the right direction. We have just been entering the true endmill size in HSM for our router because we pretty much only use one tool and it is simpler that way.
My preference is 2D Adaptive Clearing with a finishing 2D contour profile. Adaptive Clearing is designed to keep a constant chipload (horsepower requirement) and is great at maximizing the smaller machines. You can also add pre-drilled holes in HSM so that you aren’t always boring with the end mill.
I would try to take a more agressive cut on the PCNC770. I am not an expert, but I would plug in 6500 RPM, 0.2" WoC, 0.250" DoC, and 0.003 IPT to see what feed rates you can get (it should be around 39 IPM). CAUTION: Remember horsepower isn’t calculated in HSM. I think this calculator and this reference site are a good starting point. Based on those calculators, it is right around 0.95 HP assuming an 80% machine efficiency. it is worth taking a few test cuts starting at 60-75% feed rate (of 39 IPM).
If you have a spindle meter or ammeter, see what the spindle load is during the cuts. It may be counter-intuitive, but you want to take a more aggressive cut. Aluminum is very forgiving, but in general too low of feed will serve to dull the cutting bit since it is work hardening the surface and not removing material quick enough.
We bought some Lakeshore Carbide 1/4" 3-flute ZrN coated roughing/finishing end mills to use on our Taig CNC mill. They are a work of art and I am anxious to test them out.
Are you aware you can also get HSMWorks as well? This would only be useful if you needed 3D profiling (maybe some awards or making molds for casting urethane??).
Are you planning to press-fit the bearings? If so, I would do a 1.124" hole.
Enjoy the machine and be sure to share some photos of what you make on it
Bore to a slightly deeper depth, if that’s possible. or just take the film out with a deburring tool.
It might be due to the wall thickness being slightly larger, like 0.127", or the metal flexing out of the way.
On the first question, I’d be willing to bet your running a roughing process for the bearing hole and it needs a finishing process to remove the remaining material.
In the second scenario, I’ve experienced this quite a bit on my tormach. I would either use a deburring tool to remove the foil, or set my zero for the Z axis a tad bit lower than actual zero. This happens sometimes based on how the workpiece is clamped down, which can cause the material to bow in the center, or pick up on one end.
Maybe this is a function of how HSMExpress works, but I don’t really understand why this is even a problem. Aren’t you hand entering a depth to cut to? Or is it selecting that depth based on the depth of the chain you selected?
If it’s the former, just put in -.1875 or -.250 for a .125" wall thickness tube.
HSMExpress selects the depth of cut based on the contour/profile you select. So, if the part being milled is modeled with a wall thickness of .125", but in reality has a wall thickness of .127", in a perfect world, the milling operation leaves .002" of aluminum at the bottom of the hole.
What I have found is that if I just set the “Bottom Height Offset” to a value of .010", then the end mill will extend .010" beyond the selected profile. This will cut the hole cleanly as long as the material being milled is less than .010" thicker than the expected .125".