[Sanjuro82]

Howdy everyone, new member here from Bryan Texas. Glad to be a part of this community I'm sure I'll learn a lot by reading through the threads on here. Hopefully down the road I can be of help to someone else.


Anyways my current dilemma is with engraving on anodized 7075 aluminum. I'm a currently using this V cutter (from MSC) for engraving with various levels of success. The main problem is that I'm engraving forged AR15 lowers which vary slightly from one to the other. So I have to spend ton of time leveling and adjusting the lower in vise so I can get a consistent depth of cut. If I don't get things just right the results are pretty poor.


I'm thinking of purchasing a some type of spring loaded engraver (drag or rotating) which I assume will help with the variances between parts. But not sure which type to go with. Should I go with something like a 2L spring engraver? Or should I use the drag type? Can I can I run the operation multiple times with the drag to cut deeper? Or are there other options out that I'm not aware of? All the parts that I engrave will be painted so I need to be sure that the engraving will be clearly visible/readable after the painting.


I'm currently engraving at a depth of 0.01 inches. My text height is 0.13 inches. I also have a logo that I engrave that is approximately 1.25"x1.25".


Here's my set up
Tormach PCNC 1100
Mach 3
Fusion 360 (for CAD and CAM)
Kurt 6" Machinist Vise
Tormach 5" Vise


Also if I'd be better off going with some other type of engraving (CO2 laser, fiber laser, etc...) setup please feel free to make that recommendation. Thanks so much. All help and info is greatly appreciated!

[Mooser]

If there's enough qty of parts to make it worth doing, I'd look into making a dedicated fixture that located off the top of the parts and held them until clamped into the vise. That would eliminate a lot of your issues right there.
The drag engravers work OK
Just a thought

[quarky42]

EDIT: This post is going to be a bit long, but in it I will give you several options that you can try. Also, I take some considerable time to explain the problems I've ran into so I really hope that it helps. A fixture will not work for AR15 Lowers because of manufacturing variations. I have found out the hard way that the surfaces you want to engrave might be flat, they might be curved, they might be easy to level in the vise or almost impossible to level in the vise.

So, let me start off by saying that I have experienced the exact same problem. First, the Tormach Spring Loaded engraver will not engrave deep enough to meet ATF requirements as far as I can tell. (I have the spring loaded engraver and all the test engravings I've done, don't seem to be deep enough though measuring the actual depth is difficult.). I hear ya on leveling, it's a pain, also one of the lowers that I engraved had a "crown" on the mag well meaning if I set the z height to 0 at the middle of the magwell, it was z- a couple thou when you jogged towards either edge. That was with the mag well perfectly level... the mag well itself had a curve.

So, I'm going to talk about several methods here.... they all have their drawbacks and it's up to you to decide what you want to learn how to do.

LUCK METHOD: *IF* you get lucky and the surface you want to engrave is pretty flat, then just level it in the vise. You'll get better at doing this and yes it is tedious. Just be glad that you are dealing with a flat surface and not a curved one. If you are dealing with a curved surface (forged lower for example), then you are either going to need to account for the curve OR you are going to need to make it flat.

MAKE IT FLAT METHOD: Strip the finish off the lower, chuck it up in the vise as perfectly level as you can get it. (Keeping in mind that magwells can be rounded or at an angle...this is a booger to deal with) and then lightly mill the face that you are going to engrave flat. Once it's perfectly flat, you can engrave anything you want into it and it will look great. Lightly polish or sandblast the side you milled to make the surface finish match. Optionally lightly sand or buff the lower (if desired). You might as well cerakote the lower at that point and give them back a lower that is any color they want and has a really nice finish to it. You'll have a fair amount of labor and the cost of refinishing to factor in... but it will be done very precisely and it will be finished in any color the customer wants when you are done. The key here is to mill off the MINIMUM amount of surface material to make the surface flat AND making sure your machining marks that are left behind are cleaned up or as minimal as possible.

DIRTY METHOD: The quick and dirty...and I mean DIRTY way to do it, is to break your engraving up into sections and manually change the depth of each section to compensate for the variation in your piece. (That is assuming you can at least get the piece level in one direction, but I have found that even if you get the piece perfectly dialed in, you can still have a "hump" in the magwell.) Setting up your cam so that you can split up the code like that might be problematic, but something like lettering might be okay to do it in "segments" of 3 or 4 letters at a time. This is time consuming and can be messy and the more you mess with your z axis the more chance for error. I know from first hand expensive experience about this... so this may not be the most ideal solution for you.

SKILLED METHOD: (This method will take the most skill and time to learn on your part, but once you've learned how to do it, you can probably engrave just about anything as long as it can be modeled / measured.)

Watch this: https://www.youtube.com/watch?v=4XxLTsXr7m8
It relates to what I'm going to recommend and it would help if you see where I got this idea. Yes, he's engraving a barrel, but pay close attention to the technique that he's using. He's approximating the surface of the barrel in CAD and THEN applying a 2d curve to that surface for the engraving tool path. That is, in my humble novice opinion, the best method to learn and has the fewest drawbacks even though it is challenging.

First: Take some measurements and modify your engraving surface model to match the angle of your receiver. Then your g-code will be tailored to the receiver itself. A short / rough version is this: Load the lower receiver in the vise as best you can. Level it as best you can, but spend less time leveling it and more time measuring it. Once the receiver is loaded in the vise, take a tool like a touch probe or a Haimer gauge (or any kind of accurate touch off gauge) and measure the area to be engraved at different intervals. Let's say you are going to engrave within a box that is a certain size... let's use your dimensions: 1.25" x 1.25" and 0.13" x 1.9" long (that 1.9 is estimated, but you can fit that nicely on the mag well for example)

So for the 1.25" box, take at minimum 9 measurements. ([0,0,z1] [0,0.75,z2] [0,1.25,z3] would all be up your y axis for example...then you'd take measurements up the center of X (X=0.75)for the same Y values and again for X=1.25 for the same Y values... in the end you'd have Z1 through Z9...a set of Z values at every location. You can apply these Z values to a surface (or surfaces) in CAD and then base your engraving off that. You'll need to keep track of what you are going to use as Z=0... what ever you set your Z=0 to on the lower receiver itself in the vise will need to be your z=0 on the CAD drawing for this method to work.

Now, if you could model it as round piece with a really huge radius, that would make it a lot easier. In Fusion 360, they do have a sculpt mode you can get into, so I would be tempted to play with that and push or pull those points up or down as needed and then place my engraving on that surface. You are basically modelling the surface as it exists in the vise. The first time you do this, it's going to be a pain in the a$$. The second time you do this, it's going to suck. The third time you do this it is going to suck a little less. By the 10th time you do this, you're going to get better at it and you'll eventually be able to do it very easily. For me, the hard part is learning how to make Fusion 360 (or your CAD of choice) create the manipulated / offset surface that you want.

While I don't have all the answers on this last method, this is exactly what I plan on doing next time I need to engrave a lower. It's going to be a pain to learn, but once I can model a surface that is in my vise based on some data points, it'll be a VERY valuable skill. I would rather spend 45 minutes taking measurements than spend 30 minutes "sort of" getting the lower receiver level and still having error because the receiver isn't perfectly level and it isn't perfectly flat.

Let me take a step back and say one thing though: At 0.01" deep, you're engraving deep enough that even if you have a variance of 0.004" in the thickness of your piece, as long as you pick a good starting Z height... you should maintain proper ATF depth. The quick and dirty engraving that I did...thankfully, the lower was pretty flat...only a slight variation in it... so when I did my first pass, it came out too light. It was cut fully into the lower, but not to the right depth, so, I raised by Z reference height by 0.003" and ran the program again. (I basically told my controller that when the mill head was 5" above the part, I adjusted it to 5.003" instead...so, when I re-ran the code, it went 0.003" deeper into the part on the second pass and this ensured that I was well past the 0.003" minimum required by the ATF. This method worked, but on the second lower that I did.... I found that the middle of the magwell was "humped" and there was a 0.003" difference between the middle of the magwell and the outer edge of where I was going to be engraving. So, I just reran the portion of code that covered the second half of the engraving and reran that again 0.003" deeper. I can tell what happened when I looked at it, but it still looked pretty good. This was definitely a dirty way of compensating for the problem, but it got the job done and the person it was for was very happy to have it done.

[AUSTINMACHINING]

I use the spring loaded engraver from Tormach. Works great on anodozed aluminum.

[quarky42]

I use the spring loaded engraver from Tormach. Works great on anodozed aluminum.

It's pretty, but when you're engraving on an AR15 Lower Receiver, it's likely for ATF markings which have to be at 0.003" depth or deeper. The spring loaded drag engraver isn't that deep.

So, yes it'll engrave, but it likely won't meet requirements which would be bad if you're making a sbr lower receiver that you have $100 into the lower and $200 into the tax stamp.

That's why I said it wouldn't work. Not deep enough, unless I'm mistaken. Hard to verify the depth of a super thin line like that. I have the drag engraver and like it for what it is.

[Hirudin]

Looks like quarky42 has the bases covered. I have a small idea to add. A cutter with a sharper angle would make the variance in depth less apparent. With a 90° mill, 0.010" in depth will equal 0.020" in width (the depth to width ratio is 1:2). With a 60° bit, the ratio would be closer to 1:1 (1:~1.15). So, with a 90° bit, any error in depth gets doubled in the width, but with a 60° bit the error is amplified less, so I imagine the error/unevenness would be less apparent.

[edit]Darnit, I only looked at the picture of the bit you linked to. Sorry, I thought it looked like a 90° bit, but I see that the angle is clearly listed as 60°.[/edit]

[sin_arms]

I have this and it worked pretty good for the little that I used it, I just haven't used it much since most of my engraving is one off. I think I might actually sell it just because it sits around and takes up a tool holder.

Mini Spring Loaded Engraving Tools Engrave with a CNC Machine, 3-8 inch diameter

[Sanjuro82]

Wow thanks for the excellent responses! Very informative post quarky42. I'm looking into apply some of those techniques. Sin_Arms I sent you a PM about your engraver.

[shred]

Hard ano on AR lowers can chip like mad with diamond-drag (yes you can get to .003"+ deep with a few passes of drag). Rotary can be a bit better if you can get the RPMs up.

Before we got a laser the easiest way to do uneven surfaces was to break the engraving up and just delete out the letters/lines that were deep enough, move down a skosh and repeat.

YAG or Fiber Laser is where it's at but given as where you are, there are at least one and I think two high volume AR laser shops within 100 miles so unless you need something special for yourself, you may be better off just having them do it. It takes a long time to pay off a $20K laser at $40 a throw.

[inthebay]

For additional depth on the drag engraver you can run multiple passes.