Rate my rig .... teach me please

[CandL (Carl and Lynn)]

I am venturing off into cutting metals on my 1F Foreman, with the stiffy option. While I am a Mech Engr., I am not a Machinist. So the Machinists out there bash away

I have a 3 HP (2.2 Kw) ISO-30 spindle, mounted to the Z gantry via an aluminum plate.

The machine is mounted to a ¾ in ply torsion box that sits on a 2x6 wooden frame. The table has a sandbox with brake rotors and sand to help dampen vibrations.

Hopefully I achieve a reasonable level of stiffness and vibration control.

My compressed air runs through a Frankenstein air cooler/ dryer.

I have added a simple air blast system that is manually turned on/off. It runs at 30 psi. This hopefully does two things:

- removes chips so they are not re-cut

- helps keep the stock cool.

To also aid in keeping the stock cool I spread a thin layer of “tap magic” cutting fluid on top of the stock. I don’t want to mist because of the MDF.

All of my jigs/holders are ¾” MDF. It is cheap and disposable. I have “reserved” the front right portion of my machine for metal work. To isolate the space I have this:

The brush seals sit in a custom 3D printed holder. Just trying to keep the chips corralled.

Currently I am making brass name plates.

My machining holding system is based COMPLETELY of of machine coordinates. By that I mean I am setting G54 off of machine coordinates not a touch off… Ok Z is still a touch off.

To create the bottom plate I screw down the MDF, set G54 and cut out a pocket of 0.92” this is my stock thickness. The size of the MDF has to be close as in .25” but letting the machine cut the pocket insures it is correct.

To mount the stock I use the super glue and tape method, aligning the stock to the left hand side of the pocket. I also align the bottom of the stock to the bottom of the jig with ~1/64 overhang, any extra stock is machined away. Better to waste a bit than to come up short.

I then knowing where the stock run my cut out program. Part number two uses the same program AFTER I reset G54s Y to a new value. Rinse and repeat… making sure the part is cool to the touch. Melting tape is not a good thing.

This has my blanks cut. To actually engrave I made a secondary stock holder I again I used MDF and pocketed in the name plate.

The trick here to get repeatable positioning of the jig holder. To accomplish this I use .25 dowel pins. I machined .25 inch holes in the top of my base jig and then .25 inch holes in the bottom of my nameplate jig. Putting the dowels into base jig then the name jig registers correctly. Notice I said dowel pins and not gage pins … I have a few gage pins but those guys are expensive (I lose things) and dowels are close enough.

A question was also about bit selection. For this job I am using Lakeshore Carbide’s, they had been recommended by a few folks.

1/8" CARBIDE STUB END MILL AlTiN COATED 2 FLUTE ($8), I went with a stub mill because they:

- Cheap … learning I may break them

- My stock is 0.092 thick PLENTY of cut length

- Consistent diameter and short shank

20 DEG PER SIDE TAPERED ENGRAVER, .020 DIA BALL, 2 FL HP-HLX, 1/4 SHANK (Double ended ~$23)

- Pure and simple recommended by John Saunders of NYC CNC, Saunders Machine Works and Business of Machining Podcast

So there you have it, my set up for thin metals.

For thicker stock I would likely go with a SMW fixture plate and their Mod Vices, but hard to justify those now.

So my machinist friends out there, what can I do to improve? Where am I being stupid?

[MikeXYZ]

Nice setup.

I recommend switching to 1 flute end mills. Our routers have a hard time spinning slow enough. One flute end mills help alleviate the problem.

Likely, you will find metal chips everywhere. When I run aluminum, the chips fly up to 8 feet away from the machine. Somehow they end up in my bedroom, car, couch cushions… etc….

I have had poor experiences using CA glue and double sided tape, for me, the coolant had a tendency to interact with the adhesive, and parts would release prematurely. I prefer mechanical fasteners.

The coolant can be controlled through M commands via Gcode. It’s worthwhile getting that to work with a pnaumatic solenoid. Each time you forget to turn the coolant on could snap a cutter!

[CandL (Carl and Lynn)]

Some really nice thoughts. thanks for the suggestions.

Here are my thoughts:

• Agreed chips fly everywhere, the brushes do seem to help a lot though. Right now cleanup is a broom and dust pan. I am considering a cheap shop vac and mini cyclone set up to vacuum up the chips. What do you use?
• I am running air blast only with no coolant. Ok I lied a bit there, I smear the tap magic onto the top of the stock, figuring it can’t hurt. But “coolant” never really touches the MDF or tape. As far a pneumatics for my air blast that maybe a future consideration, but right now just simple.
• I prefer mechanical fasteners too, but with thin stock they can deform material. My pocketed MDF is kinda, sorta a soft jaw set up. I tape the top just to keep the Z constrained for engraving. I don’t see engraving generating high loads on the clamping system.

And now the deep dive into the weeds … In general I like the single flute or “O” endmills for just your reasoning. I am using a 0.125” (1/8) endmill in C260 brass …. this is how I run the numbers.

Brass recommended SFM is 250-350 with Carbide tooling. RPM=(SFMx12)/(Dia*Pi) .. at 10000 RPM I get 327 SFM right in my range.

Recommended feed per tooth is 0.0007-0.0015 so IPM = RPM * Number of Flutes * FPT. So my feed rates are:

for 2 flutes, 14-30 IPM

for 1 flute, 7-15 IPM

These number seem reasonable to me.

I would switch to single flute when I can’t feed fast enough.

The other issue here is chip clearing. I like 2 flutes as the gullets are still fairly large, I also like the symmetry of the bit for a bit more rigidity. I certainly would not go to a 3 or more flute design.

Does my logic make sense? I am an engineer so the equations make sense to me, but I lack a “gut instinct” to tell me thumbs up or down.

[Ken5]

The O flute is better because aluminum is sticky and a single flute allows the chips to evacuate without galling up the bit like 2 flutes seem to do.
I agree with Tap Magic best thing ever for aluminum cutting

[CandL (Carl and Lynn)]

I was really worried about “sticky” and galling but I am just not seeing it on the .125” Maybe the Aluminum Titanium Nitride (AlTiN) is helping. Now granted I have cut less that 10’ of slots … guess time will tell. (10x loop inspection)

[joejk]

Carl

I think you did a wonderful job putting together a nice set up to cut name plates from brass. All of the math and thought about repeatability is all good. The input from Mike and Ken has logic to it too.

In my later years now as a machinist I have learn one important thing is try to use the KISS method - Keep It Simple Stupid.

I can tell Carl is an engineer by his thought process which is good but lacks the gut feeling its right. I have come to the process as to just try a few ideas and analyze the effects or results of the project and use the one that works the best.

I don’t do the feed and speed math no more but have general thoughts, about feeds and speed for many common materials just in my head which I have trained my brain to go through a project in my little brain(computer screen seeing it run).

A lot of the feed and speed stuff is more by sound and vibration of the machine rigidity and the cutter sound. This is how I determine how hard to push the set up. Once you hear the right sound then you have a base line for any project.

Of coarse there is the time factor but in my head time factor is not important to me but the finish looks of a project is important to me. Over time you will be refining the feeds and speeds for each project and when you come back to a similar project you will have a starting point to test other things but always have the gut feeling of were to start and decide if you want to speed it up or not.

As far as coatings or no coating is up for discussion on what is best for what materials. I have found that the TiCN is a good general purpose coating that works for most materials, wood included. Only other coating I like for brass or alum. is the ZrN coating.

Here is a source for tooling and here is a page with charts for the various coatings and materials. I have bought a lot of end mills from this site and prices are reasonable if you stay on the small size.

Now here is the website so you have some more starting points of feed and speeds for various materials. Now don’t over think it or try to do to much math just try and analyze the sounds and finish. The hardest thing can be which way to go up or down, believe me if you go the wrong way it will tell you. There is a lot of good info there but don’t over think it - KISS - !

I have no affiliation with this source but found it many years ago just to fill my needs for my little hobby shop. Also this is more metal tooling source and not so much as a wood working source but the tooling does work in wood.

Milling Speeds And Feeds: Charts & Data

Cheers

Joe

[HardtailSr (robert mainville)]

I make these clamps. they are ultra low profile . They are very strong and are sold as a set with four clamps and a tightening tool as well as three sets of low head screws for a range of materials from 1/4” to over an inch thick with others available for even thicker materials. as to cutting the aluminum I have a 220 volt redline spindle i am cutting them at 15000 to a depth of .015 each pass with a 1/2 inch cutter single flute bought on amazon for about 30 dollars. so a lot cheaper than some of these CNC bit companies. These clamps pretty much guarantee you are not going to hit the clamps and ruin a bit and the work. “you can’t hit what ain’t there”

[CandL (Carl and Lynn)]

Yup guilty as charge …give an Engineer and an equation and we are off and running. I will say that I learned the process from Cincinnati State where I took classes with 18 yr olds. By the way the courses were free. In the USA most states require colleges that receive state money to offer classes to people over 60 for free, no degree but lots of knowledge.

So for grins an giggles I gave the AI a shot at this … actually 3 of them. This is what MS CoPilot had to say:

Prompt: “I am machining C260 brass on a onefinity elite foreman with the stiffy option. My 3Hp spindle has a max rpm of 18000. I have air blast, but do not have coolant. I will be using a 0.125" endmill with AlTiN coating. I will be doing slotting and profile cuts. Am I better off with a one or two flute endmill. And then what should my feeds. speeds and depth of cut be. Please use imperial units”

Response:

Use a 2-flute carbide endmill for C260 brass. At 10,000–18,000 RPM, aim for 0.001"–0.0015" chip load per tooth, with feed rates of 20–54 IPM and depth of cut between 0.010"–0.035", depending on operation.

Why a 2-Flute Endmill Is Better for Brass

• C260 brass is free-machining and doesn’t gum up like aluminum.

• A 2-flute endmill offers:

• Better balance and rigidity than a 1-flute

• Higher feed rates and improved surface finish

• Adequate chip evacuation, especially with your air blast setup

Avoid 1-flute tools unless you’re cutting very soft materials or need extreme chip clearance.

Feeds & Speeds for ⅛" (0.125") AlTiN-Coated Endmill in C260 Brass

These values assume a rigid setup with the Stiffy mod, air blast, and no coolant. Start conservatively and increase feed or DOC as needed.

Additional Tips

• AlTiN coating is fine for brass, though not ideal—uncoated or ZrN is better. AlTiN can cause slight edge buildup in brass, so monitor finish quality.

• Use conventional milling for slotting to reduce tool pull-in.

• Avoid rubbing: If chips are dusty or the tool gets hot, increase feed slightly or reduce RPM.

• Use a short flute length to minimize deflection and maximize rigidity.

Sources:

Hmmm, Notice the 6gtools …. go figure.

All 3 AI came up with about the same recommendation. Gemini actually showed the same steps I used.

Do I trust them not yet, but as quiet second opinion they are worth the keystrokes. (It called C260 “free-maching” it is not, C360 is however)

I am using the “stubby” endmill so yup a short flute and shank length.

Anything that keeps me from being stupid is good thing.

[MikeXYZ]

While I went down a similar rabbit hole, I noticed that a lot of recommended feeds and speeds, especially from AI, are very very aggressive.

I reasoned that this is the case because tool manufacturers post recommended feeds and speeds for a production environment. The recommendations they make are based on the assumption that you want the absolute highest material removal rate possible. I believe this floods the internet with high feed rate recommendations, and AI responds accordingly.

Perhaps try asking AI to recommend feeds and speeds, but tell AI you are new to metals, are using a hobby machine, using “light” workholding techniques, and would like to stay on the conservative side.

[CandL (Carl and Lynn)]

I believe we are pretty much in agreement…. I did say use them as a second opinion. I like the using “light” work holding techniques, I will add that to the prompt.