CNC Process, a step by step walkthrough

[b0gh0s]

OK Gang,

Seems to be a mix of newbies and chipmaking veterans, I thought I'd post one way (not necessarily the right or only way) to make a part from design through small CNC production.

First the equipment/software list:

CAD: Autocad 2002

CAM: RAMS 3D Gold Edition

Motion Control: Mach3

CNC Mill: Taig 2027ER customized with VFD drive 1/2 hp motor, flood coolant on xylotex control board and 270oz/in steppers.

CNC Router: K2 14x26 Bed 3 axis using 3/32 carbide fish tail burr.

Tooling: Misc Drills, 5/32 2 Flute and 4 Flute End Mills, 1/16 2 Flute End Mill, vises, steel and aluminum stock, etc.

[b0gh0s]

The part I'm working on currently is a replacement for the Turbulence, Evo 90, and Evo 50, (all use same plastic part), anti rotation guide. The plastic one gave me troubles in a few places,

1) it's plastic
2) it breaks if you flex it to remove the swash and main shaft all assembled
3) it can be a pain to get in and out of the frames because the frames are fairly tight.

I wanted to design an aluminum and carbon fiber replacement.

I'm including a 3D pic to show the overall concept.

http://www.helifreak.com/attachment.php?attachmentid=102125&d=1245216879

[PittJitsu]

Hi. I too am a machinist. Proud owner of an old school Bridgeport mill. That's a very nice piece. I'm new to RC's and helis all together. Has anyone tried using Ti for any of the parts? I keep wondering what I could make out of the titanium I have around.

[b0gh0s]

Since in many cases it is easier to develop the code to machine a part from 2 D drawings, we'll start with a simple 2D part drawing that is precisely drawn to dimension.

The pic below does not have dimensions written in, because the CAM software doesn't need them.

[b0gh0s]

Hi. I too am a machinist. Proud owner of an old school Bridgeport mill. That's a very nice piece. I'm new to RC's and helis all together. Has anyone tried using Ti for any of the parts? I keep wondering what I could make out of the titanium I have around.

Titanium is great for shafts and stuff like that, not sure it'd be real practical for frames or bearing blocks, but if you have the means and time, it sounds like an interesting project....

[b0gh0s]

Once the 2D drawings are done, you need to go through them and make sure of a couple of things:

1) lines are exactly drawn to dimension, since most stuff is in metric, thats usually how I measure but convert to SAE since tooling and machining with the equipment I have is easier that way.

2) All lines on shapes or outlines need to meet/mate and connect properly, otherwise the CAM software will treat it as a set of discrete lines.

3) Make sure the part is centered or edged to a known reference point, I make all of my parts assuming the bottom left corner is 0,0 in the XY plane

[b0gh0s]

Next step is to think through a machining strategy. This is the part where CNC machining ceases to be a science/computer project and becomes a true art form. Machinists with many years of experience and chips made measuring in the tons are much better at this than I am but I'll do my best to describe some of the challenges and a few commons solutions used in this project.



1) Parts have to be held securely to be machined cleanly, machines can't magically cut a part from a block of aluminum since in many cases the cuts require the part to be open, closed, or both.

2) 99% of the time you can't run a single operation to make a part that has any complexity to it at all.


Since this project consists of multiple parts, lets start with the difficult one first.


The aluminum block has machined surfaces in nearly every dimension which means we'll have to fixture, machine, refixture, machine more, lather rinse repeat.

For this part my strategy is (based on experience and knowing what will work reasonably on my machine) will be as follows at a high level:

1) Rough cut a blank block of aluminum from 2.5" wide 1/4" 6061 aluminum stock that I have in bulk. Cut it to a 3" length which should allow cutting 6 parts from a blank.

2) Square off and pre-drill and tap a steel fixture block to be used to hold the parts while profiling them out of the aluminum

3) Fixture the aluminum predrilled blanks to the jig block and profile cut out 3 parts at a time. The 2.5" wide block will be predrilled twice (once on each side) so once 3 parts are cut, the remaining block can be secured to the fixture block and another 3 parts can be profiled out. Since the parts will be fixtured flat, we can also drill the holes to be tapped for 2mm screws with a tool change.

4) Once profiling and drilling the 2x 2mm mounting holes is done (and we'll do a bunch of parts this way), we'll flip the block on it's side, hold in vise (with the part butted so we can accurately locate 0,0 in the cartesian plane on the mill), and drill the two side holes that will be tapped for 3mm screws. This needs to be done twice per part (once on each side) with two holes per operation.

5) Flip the part upright in the vice (on a steel parallel) and slot mill the top using a 1/16 end mill. Since 1/16th is slighly smaller than the carbon brack we'll be using (which is .076 thick stock), we'll have to do a few passes.

6) Once all milling and drilling operations are done, deburr the part with a Shaviv tool.

7) Use a tapping head setup on my drill press to tap the 3mm side mount holes.

8) Use the tapping head to tap 2mm holes for mounting the carbon bracket

9) Open up (using a hand drill) one side of the 2mm holes so that the screws will clamp the carbon bracket

10) Manually finish the parts with sand paper (lightly) to shine up the front/back surfaces.

[b0gh0s]

So that all sounds easy enough right? Lets get started.

1) Rough cut a blank block of aluminum from 2.5" wide 1/4" 6061 aluminum stock that I have in bulk. Cut it to a 3" length which should allow cutting 6 parts from a blank.

I buy aluminum in 12ft lengths from a local supplier, one of my staples is 1/4" thick 2.5" wide 6061. I use 1/4" because it is just over 6mm thick making it perfect for most applications where you need a part that can be held by a 3mm screw.

I buy it 2.5" wide because that width fits a variety of purposes and is also about as large as I can easily hold with small vises on the milling machine I have.

We'll use the metal bandsaw to chop a few 3" lengths, the cuts don't need to be precise this part usually goes quick...

[b0gh0s]

2) Square off and pre-drill and tap a steel fixture block to be used to hold the parts while profiling them out of the aluminum


This part is tedious. Making a fixture block is only a one time activity per part but always seems to take the longest.

I'm going to start with block slightly bigger than 3" x 1.25". The thickness is not critical, I have some bars of 5/8" thick hot roll steel that machines fairly well.

The idea here is to get a reasonably accurate starting point, the exact dimensions in this application are not critical since we'll be machining from a common reference point. First, I use a 3/8" end mill and chuck the steel in a vise squared to the machine with a dial indicator, (meaning the vise is perfectly squared to the mill column to within 1-2 tenths of a thousandth (+/-.0001).

Using the mill I edge off the steel block with a few passes to get a nice finished edge on all 4 of the edges. This way when I re-vise the block on parallels the next time, the block will be squared in the vise.


Now we've got a reasonable starting point. I've determined that I can hold the block with it's top face above the top edges of the vise I'm going to use with enough clearance to allow me to machine into it without hitting the vise jaws if I prop it up on 1/2" parallels. I do this and get the block edged into the vise and clamped securely.

Using a vise stop bar (which will be visible in pictures to follow), I butt the bar against the block to allow me to quickly re-insert the block on the parallels and not have to reset the CNC machine 0,0 for X and Y.

Speaking of which, I now use an edge finding tool in the CNC machine to find the lower left corner of the the fixture block that I've made and vised, to setup the machine 0,0 reference point.

Now the lower left corner of the block is referenced in the machine as 0,0, I'll also set the machine default height at the top of the block face temporarily as well.

[b0gh0s]

Pics:

Squared off steel fixture block, and the block vised in the mill touching off the X axis 0 point (to the edge of the block).

[lex7919]

Hey, Very cool thread nice one im enjoying this bringing it all back slowly! im sure many people will think the same as i do so keep it up :thumbup:

[My 2 Cents]

:noteworthy Keep it up :thumbup:

[b0gh0s]

Next step in process 2 is to figure out where the parts are going to be fixtured onto the block and machine the steel block for it.

Plan is to do 3 parts. I'm going to use 2 x 3mm screws per part to hold it down to the steel fixture block. The parts are going to be machined starting at 0,0, 1,0, and 2,0.

In the drawing there is a cutout in the middle of the part, since that can be done as a secondary operation, I'll put the two 3mm screws in that area of the part and machine out the cutout later (thus removing the fixturing holes).

The picture below illustrates where I placed the mount holes on the part (in red).

[TMoore]

If it were me I would just chuck the block in the vise and mill the part to a depth a few thousandths deeper than the part will end up, slot it with a slitting saw, then flip the part in the vise, mill off the top and tumble it. You'll need a few more ops to do the tapped holes but that's no biggie.

Am I missing something?

TM

[b0gh0s]

Not sure I'm reading it right but if I profile the part out of the aluminum with the alu block just gripped in the vise and let it drop out of the bottom I've always gotten really poor results on the edge finish on the profiled surfaces. Is this what you are talking about Terry?

[b0gh0s]

If it were me I would just chuck the block in the vise and mill the part to a depth a few thousandths deeper than the part will end up, slot it with a slitting saw, then flip the part in the vise, mill off the top and tumble it. You'll need a few more ops to do the tapped holes but that's no biggie.

Am I missing something?

TM


And I am going to use a slitting saw instead of end milling the slot.

What I'm doing is setting up to profile and cut 3 of these at a time, makes production of more than 1 part a lot easier. I'm back documenting this as I've finished a bunch of the operations already, I'll get there in a few posts :D

[TMoore]

Don't drop it out of the bottom, leave a little to hold on to in the vise and then flip the part, mill off the back side and profile around the backside with a chamfer or radius cutter for deburr.

TM

[b0gh0s]

Got it Terry. To do that, I'd need to machine the alu block with a nice edge so I can flip the block and re-locate it. Also, I'd need to mill exactly in the middle of the block so that when I flip it, the part is centered, meaning I'd also have to finish the block edges.

My mill isn't big enough to do clean surface or "deck milling" with any efficiency which I think yours can do pretty well based on our offline conversations.

This method I'm using will look really familiar when I show the pics, I think I've seen you use a similar method on some parts/pictures :)


Also, I want this part to be almost exactly 0.25" until after I peck drill the side mount holes so that they are centered on the side of the part.

[b0gh0s]

So back to the fixture block:

Now that I know where to drill some holes I'm going to drill 3 pairs of holes in the fixture block so I can make 3 parts at a time. Based on the picture and assuming the fixture block lower left corner is still 0,0 I'm going to drill holes in the block in 6 locations:

X0.2214, Y0.6391

X1.2214, Y0.6391

X2.2214, Y0.6391


So these number may seem a bit precise. What I did was center the holes in the drawing and the center of the curved cutout radii and Autocad gave me those dimensions. Frankly they are not as critical as significant digits would suggest but consistency is the key so as long as the machine sees consistent numbers based on the known 0,0 location we set by "touching off" the fixture block above, we'll have consistent results.

To drill these holes, I'm going to tell the machine to do a "peck drilling" operation which for those who don't know, as the name suggests, means the machine will cycle the Z axis (the head spinning the drill bit) up and down in increasing depths to "peck" away at the hole to get it deep enough. This will give it a nice clean hole, increase the drill bit life, and not load up the machine unnecessarily.

Since I've decided to use 3mm screws (which I have an abundance of as a result of the helicopter hobby), I'll need to drill holes that are 0.098" in diameter so I can tap the holes for 3mm x 0.5mm threads. For drilling and tapping references, do a google search, there are a number of tables that will give you exact suggested drill diameters for holes to be tapped.

Since the point of this thread isn't to teach G & M codes, I'll spare the gory details but lets say at this point it's easier to code a peck drilling opp by hand and that I've written the code. Video below is an example of peck drilling on my machine, it actually shows the peck drilling of an aluminum blank which we'll talk about in a following post.




YouTube - Peck Drilling Example

[b0gh0s]

Are we having fun yet? Of Course!

Just so you all don't think I'm superman, I've been cheating a bit here and am back logging stuff I've finished already. That said, lets move on a bit.

Now that the fixture block is drilled, I use a hand/manual tap since it is only 6 holes and in steel with no "through" hole, and tap each of the holes in the fixture block using a 3mm x 0.5 tap. Once this is done, I run a duburring tool on each edge of the block and clean it up for lots of handling.

I'm going to cheat again and post a picture of the finished block (you'll see the profiling patterns in it from having been used already, don't worry we'll get there).

[My 2 Cents]

:noteworthy:smokin:

[b0gh0s]

Now that the fixture/jig block is more or less finished, it's time to get geeky.

Since as you can see in the previous picture, we'll be doing 3 parts at a time held down in a flat horizontal position, we can get away with running 3 machining procedures on all three blocks without undo-ing the vise or screws. Here is an overview of what we will do, please refer to the pictures below for visualization:

1) Peck drill two holes suitable for taping 2mm threads into the top of the block (first pic)

2) Cut the outer profile of the part using a 5/32 2 Flute square end center cutting carbide end mill leaving about 5 thousands of extra material all the way around (.005 offset) using a 0.06 inch "downstep" pattern which means making a pass all the way around at a cut/slotting depth of 0.06", then 0.12" then 0.18", etc. Total depth of cut to ensure that we get the whole 1/4 inch part cut cleanly will be 0.27inches, (this means we will be cutting into the steel block by about 0.02" the first time we run the code, this is important to know for reasons to be explained). 2nd Picture.

3) Run a high RPM finishing pass using a 5/32 4 Flute square end carbide end mill at full depth at the exact outer dimension (thus taking off 0.005" of material on the outer profile to give a clean cut.

[b0gh0s]

So where's the geek part <giggity> you ask?

The next step here is to generate some G code to tell the machine how to perform the 3 sub steps described above.

Couple of things to consider going into this using CAM software such as RAMS requires a bunch of setup,

1) I've spent many hours loading and refining "tool profiles" that the software uses to figure out how to tell the machine to do things based on the tools I tell it to use.

2) I've spent many more hours rewriting the scripts and post files which generate code to make the machine do what I want it to instead of something that RAMS thought might be useful (and usually isn't).

3) Machine and controller specific setup is required in the software to ensure that your machine recognizes coordinates, arcs, and G code commands the same way as the software.



Lets get to it.

Opening up the RAMS tool and loading in the basic 2D drawing (shown above), we tell the tool that the stock we are using is 0.27" thick (yes it's ok to lie to the tool).

Next we choose the part of the drawing we want to machine first, by clicking on the two 2mm holes to select them, I think tell the software that I want to use a the appropriate drill (which I've setup a tool profile for), and that I want to peck drill at the center of the circles a hole going to a depth of 0.27" using 0.06" pecks. The 0.06" peck is what I've figured out (through experimentation) what my machine and the particular drills I've been using can handle safely and efficiently. I tell the machine to set the RPM at 5000 for these operations and to shut off the spindle when finished with the operation.

Next I select the outline of the part, select the proper tool (5/32 2Flute endmill) and tell the software that I want to "profile cut" this shape on the EXTERIOR of the shape, using a 0.005 (5 thousandths) offset (leaving extra material on), and to cut to a depth of 0.27" using down step passes of 0.06" increments (again trail and error on my machine helped figure this out). I tell the software that I want to feed the tool into the work at 2inches/minute and that I want to cut the profile (for now we'll change this later) at 5inches per minute at an RPM of 3500.

This is because for the first part we cut with this code, we will be cutting into the steel block on the final pass at 0.027" depth. Once we've cut one complete set, and the steel has been cut, we're going to bump up the inches/minute on cutting to 7ipm for this operation.

Finally I select the outline again, and this time select the 5/32 4 flute tool and tell the software that I want to cut the profile with no offset (we're taking off the last 5 thou of material), and that I want to feed at a rate of 15 IPM at an RPM of 5000. This is to get the metal to a fairly nice and shiny finish on the cut surface.

Once I've told all of this to the software, I tell the software to create a ".T" file which we are going to hand over to the motion control software to read.

The software (thanks to my handy scripting and programming) will now automatically generate the code to perform these operations and change the tools and tool height offsets automagically during the machining operations and pause for me to set the new tools in as appropriate. It also knows based on parameters I've given that I want to repeat this 3 times 1 inch apart on the X axis.

No pics on this part, most of it would be screen shots from RAMs which aren't all that interesting. If you wish more info on this software visit DeArmond Tool and take a look at their demos. I'm in no way associated with them nor do I specifically recommend the product.

[b0gh0s]

Next, we need to take the blocks of aluminum that will eventually be parts,
and drill some mounting holes in them.

These holes will be almost in the exact same locations as the holes drilled into the fixture, I say almost because I learned a while ago, that you need to leave material ALL AROUND a part to machine off if you want an accurately sized part.

Therefore, we'll take the peck drilling code from making the fixture block and modify it so that we move the y axis point UP 0.01 inches. What we'll do is then put the aluminum block into the vise in almost the same position (exact corner edge is not critical) and tell the machine to follow the drilling code and drill 6 holes of 0.120 inches (just slightly larger than 3mm) in the same locations as the fixture block so the holes will line up (except leaving extra material below where y=0 so that the bottom of the parts gets machined too).

Now the video below shows this being done.

If you look closely you'll see the aluminum is fixed in the vise and the machine is drilling a series of holes that as we'll see momentarily will allow bolting this hunk of metal to the fixture block.

YouTube - Peck Drilling Example

[b0gh0s]

Now that these holes are drilled and we have the code for the first set of operations, we can bolt the aluminum blank with the holes in it to the fixture block, set the fixture block in the vise located at 0,0 (basically butting against the steel bar you could see in the last video and up on a set of parallels). These locations have all been manually set in the machine and then in the code so that the machine understands that the top of the aluminum block (which is 0.25" above the original 0 height we set to drill the fixture block) is now the new 0 offset.

In the G code, offsets are called as things like G54, or G59P12, etc. Essentially the motion control software (in this case Mach3 by Artsoft), remembers specific coordinates in the X, Y and Z plane where 0,0 would be set for a specific fixture, vise, or work location. The machine has a "zero" function where it uses limit switches as a reference point. When you tell Mach3 to "Home", it runs all of the axis until the switch for each particular axis is tripped and thus resets it's home location. The offsets are literally a delta distance on each axis to a particular location on the work table from that home point. This allows the machine to run, be shut off, turned on, homed quickly, and re-used again to do the same operation without having to run "touch off" operations and edge finding (which can be painfully slow) each time you want to run the machine.

This is useful in our case since I am planning to run the machine through the operation we just setup at least 8 times making a total of 24 parts.

Pics and vids are worth a thousand words, so here are some.

First, the machine peck drilling the 2mm holes (the two pictures)


Then a few videos

This is the rough profiling operation using the 5/32 2 flute end mill. Notice the coolant and the resulting mess hence the large plastic tub under the mill.
YouTube - Machining part profile


This is the finishing pass at a higher speed
YouTube - Finishing Pass



Then the last two pictures of the finished parts on the jig block ready for removal and the next operation.