HSM Express+Tormach undersized holes

[billbo911]

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.

[josesantos]

Originally Posted by billbo911

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 1100 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.

I'm downloading HSM Express right now, but I'd suspect there might be something wrong with your cutter compensation settings. Either that or some setting to leave stock on walls.

[protoserge]

If you are running 2D Adaptive Clearing without a finishing contour pass, you would see this. Look under the "stock to leave". The default "stock to leave" is 0.020. So 0.020*2 sides = 0.040"

Would you mind sharing your file?

[cad321]

Is the 1/2in cutter you're using actually 1/2in? Do a quick check to make sure the cutter is worn or just undersize with a pair of calipers.

[thinker&planner]

Originally Posted by protoserge

Look under the "stock to leave". The default "stock to leave" is 0.020. So 0.020*2 sides = 0.040"

^^This.
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.

[Travis Schuh]

.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.

-Travis

[billbo911]

Originally Posted by protoserge

If you are running 2D Adaptive Clearing without a finishing contour pass, you would see this. Look under the "stock to leave". The default "stock to leave" is 0.020. So 0.020*2 sides = 0.040"

Would you mind sharing your file?

I was running 2D Pocket, not 2D Adaptive.
That said, I did look for "Stock to Leave" and sure enough, it was enabled and set to 0.02"!!! I think we found the culprit.

So now the question is, what is the best way to handle this?
Disable it?
Leave it enabled, but set to....?
How to finish it properly to size?

BTW, files attached.

Originally Posted by cad321

Is the 1/2in cutter you're using actually 1/2in? Do a quick check to make sure the cutter is worn or just undersize with a pair of calipers.

Nope, it measures .5000" (with our best calipers).

Originally Posted by thinker&planner

^^This.
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.

See above!

[cgmv123]

Originally Posted by billbo911

I was running 2D Pocket, not 2D Adaptive.
That said, I did look for "Stock to Leave" and sure enough, it was enabled and set to 0.02"!!! I think we found the culprit.

So now the question is, what is the best way to handle this?
Disable it?
Leave it enabled, but set to....?
How to finish it properly to size?

Turn it off if you're not doing a finishing pass in a subsequent cycle.

[Travis Schuh]

Originally Posted by billbo911

I was running 2D Pocket, not 2D Adaptive.
That said, I did look for "Stock to Leave" and sure enough, it was enabled and set to 0.02"!!! I think we found the culprit.

So now the question is, what is the best way to handle this?
Disable it?
Leave it enabled, but set to....?
How to finish it properly to size?


See above!

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.

[Jared]

If your Tormach has Mach3 on the control computer, I would not recommend doing cutter comp on the machine. It gets very confused with all the post processors I've used with it.

[protoserge]

Lots of good suggestions above.

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

[sanddrag]

Other folks above have beat me to offering the likely root cause of your issue, but I'll also throw this tool out there for Feeds and Speeds http://zero-divide.net/?page=fswizard

We use it exclusively with excellent results for most types of operations.

Also, I will second the necessity to use an "Adaptive" (aka: trochoidal, constant-engagement, "high speed") toolpath whenever possible when milling. It's highly preferred, for a variety of reasons.

[protoserge]

Originally Posted by sanddrag

Other folks above have beat me to offering the likely root cause of your issue, but I'll also throw this tool out there for Feeds and Speeds http://zero-divide.net/?page=fswizard

We use it exclusively with excellent results for most types of operations.

Also, I will second the necessity to use an "Adaptive" (aka: trochoidal, constant-engagement, "high speed") toolpath whenever possible when milling. It's highly preferred, for a variety of reasons.

Thanks for that! I've been looking for a tool just like this. It comes in handy when I think the Taig has HP (it only has 1/4 ).

[billbo911]

OK, next rookie question.

When milling this part, the wall thickness is approximately/ideally .125".



The pocket comes out as expected. The problem is the bearing holes. They will usually have what amounts to a layer of aluminum foil at the bottom.

Here is what I am thinking should be done to prevent this, so please feel free to correct me.

1) Mill this in two separate processes. One for the pocket, one for the holes.
2) On the process for the holes, offset the Z zero by a few thousandths.

What process, or steps would you perform to prevent this?

(Just in case you are wondering, this part is literally just for the sake of learning and has no other purpose.)

EDIT
I just found a simple answer, "Bottom Height Offset".
Set it to something like -.01" and you get a nice extension of the bit past the end of the hole, and a clean edge.

[asid61]

Originally Posted by billbo911

OK, next rookie question.

When milling this part, the wall thickness is approximately/ideally .125".



The pocket comes out as expected. The problem is the bearing holes. They will usually have what amounts to a layer of aluminum foil at the bottom.

Here is what I am thinking should be done to prevent this, so please feel free to correct me.

1) Mill this in two separate processes. One for the pocket, one for the holes.
2) On the process for the holes, offset the Z zero by a few thousandths.

What process, or steps would you perform to prevent this?

(Just in case you are wondering, this part is literally just for the sake of learning and has no other purpose.)

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.