# Fn32 Right Side Plate



## Karl_T (Feb 21, 2016)

First a bit of background.

It common for the militaries of the world to sell their small arms when they are surplus to their needs. They can be imported to the USA if dis-assembled and the receiver is destroyed. At this point it is called a parts kit. These kits are available for a great many weapons. US law requires the weapon to only be built as a semi auto NOT full auto weapon.

The FN32 is perhaps the finest example of the John Moses Browning machine gun. Only about 60 kits were imported to the USA from Portugal. Learn more about building the very similar FN30 here:
http://browningmgs.com/FN/07_FN30build.htm

This thread covers CNC machining a new receiver or right side plate. Also posted at:
http://1919a4.com/showthread.php?54588-FN32-build


----------



## Karl_T (Feb 21, 2016)

First job is get a good drawing. I'm using the left side plate as its nearly a mirror image. You need to measure everything three ways from Sunday AND then double check and then cross check it again. It takes way less time to prevent errors at this stage than to machine a part and find something out of spec. Or worse yet, rivet the weapon and find find something not quite right. (I've done that)

I measure it first with calipers and make a sketch. Then check the measurements with mikes. then check again with the DRO on the manual mill.

couple pics of this step


----------



## Karl_T (Feb 21, 2016)

Next draw it up in a CAD program. I use the free Draftsight X64. Did one layer for the outline, one for the relief or lightening cuts, one for the denial islands.
Then went back to step one and re double checked the drawing.


----------



## Karl_T (Feb 21, 2016)

The next step is decide how to machine the part.

I'll be holding a 14.85" by 4 by .25" stock in soft jaws on the cnc mill. Fist op will be just to spot drill and drill a few holes. Looks like only the return spring slot and a ruff hole at the back of the charge handle. I decided not to CNC all the rivet holes. Its actually better to just match drill these after clamping.

Next op will be the relief or lightening cuts with two tools, one to remove the bulk of the material and another to add the finish cut and all the radii. Plan "A" right now is a 1" Sandvik R390 to ruff out the bulk of the material. Then the final pass with a two flute HSS endmill custom radiused on my tool and cutter grinder.

Next step will be the outline of the weapon and charge handle slot. I'll be leaving several parts unfinished (see red lines on .pdf) so the part can stay clamped in the softjaws. These cuts will be done on the manual mill after the part is complete.

Then the part will be flipped over and denial islands cut. Right now, I'm thinking cut the backplate slot on the horizontal manual mill. This could easily be CNCed with a small endmill but a horizontal is light years faster. And I need something to do while watching the CNC do its thing. I'll also be doing the return spring slot with the manual mill.


----------



## Karl_T (Feb 21, 2016)

Next step is to write and debug the Gcode for the CNC mill. I don't own a decent CAM program, nor do I like them for the work I do. Been writing my own gcode for 25 years now.

There is a neat short cut for the gcode routes that I like. Just draw them up in the same CAD program the part was drawn in. This is mostly just copying a layer, deleting unneeded objects and then drawing connecting lines to make a route


----------



## Karl_T (Feb 21, 2016)

Then use a backplotter to convert the drawings to gcode. I use NCplot, got it for $60 back when it was developed. I've seen a free one for Mach 3 users.


----------



## Karl_T (Feb 21, 2016)

Next, write the actual gcode and test it on the CNC miil with NO tooling installed. My mill shows the route on the viewport. I included the actual Gcode for the outline cut and show a pic of the relief cut on the CNC's control screen.

i use something called parametric programming for the Gcode. That is the code has variables and loops (code repeated n times).


----------



## Karl_T (Feb 21, 2016)

THE POWER OF G41

Kind of an advanced topic, but I just figured it out and wrote the Gcode for this. G41/G42 is called cutter comp in Gcode parlance. It allows you to write the code for the actual outline and then tell the control what cutter it is using. That way you can change tooling (cutter diameter) and run the same Gcode to make the same part.

But you can lie to the control and really expand the use of cutter comp. If you tell the control the cutter is larger than it actually is, the control will offset the tool more and the part will be larger. One HUGE use of this is ruff your part out telling the control the cutter is a few thou bigger. Then for the finish pass, tell the control the right number. Now it will shave a few thou off for a perfect finish.

Here's an even more advanced trick. The relief, or lightening cut area, on the side of the RSP has a radius of 0.125". I want to make four passes each 20 thou deep for a total of 80 thou removed. The cutter route has to be farther away from the side each pass deeper. I've learned to always draw it out so a mistake isn't made. DRAW IT OUT should be the first commandment of machining.

I'm using a 0.5 inch radius or 1.0 diameter cutter for this. If the control is told these successively larger cuttter sizes, it will offset more and more to make the part just right.


----------



## Steve Shannon (Feb 21, 2016)

Very impressive work! This makes me wish I'd picked up one of the few part sets.


 Steve Shannon, P.E.


----------



## brasssmanget (Feb 21, 2016)

Hey Karl_T
I was going to suggest posting your info over here from 1919A4 but wasn't sure if you were a member here.
Then I simply forgot to ask you about it.

Glad to see you sharing the project among fellow machinists.


----------



## Karl_T (Feb 29, 2016)

Next job is getting all the tooling set up.

I use a yellow permanent marker and clear fingernail polish to ID 




Here's all the tools for the job



	

		
			
		

		
	
 ll the tools


----------



## Karl_T (Feb 29, 2016)

Next measure all the tools for height and diameter. Enter this into the control. The job must be perfect here. Or you'll schmuck a tool and make an awful crashing sound. DAMHIKT





Here I'm setting part zero. Its exactly six inched below the quill frame. 

This cnc is set up to move the knee by the part height minus the tool height at each tool change. For YEARS, I did this manually with a table written out by hand saying how much to crank the knee.


----------



## Karl_T (Feb 29, 2016)

Here's what I use to clamp the part. SOFT JAWS. You can see these have seen a lot of use from all the times the jaws have milling marks. For every use skin just a RCH off the side and bottom of the notch. Then everything is perfectly level and square.

I show some jaws for the six inch vice and another eight inch jaw is being used to clamp tight for the truing cut 






Ever need to clamp a warped part. The mill is pushing it down hard into the softjaws. You need something with give to judge how must down force there is.


----------



## Karl_T (Feb 29, 2016)

OK, time for some CNC machine porn...

Inside of receiver has the denial islands. This is required by the alphabet boys to keep full auto parts out.



Next, the part has been flipped over to work on the outside. first op is spot drilling




This is called chain drilling. A through slot for the charging handle goes here. If you chain drill first, the end mill has nowhere near as much work to do and there is a place for the chips to go.


----------



## Karl_T (Feb 29, 2016)

The most difficult part of this job is the relieved area for lightening the receiver. Had to get real tricky here. Four passes 0.020 deep, each one farther from the top edge to form a 0.125 radius. See the G41 discussion earlier in the thread




Here's the finish cut with a ball nose endmill. I got this endmill, used, off fleabay. It was chipped and worn out, So I took a diamond stone and trued up as best I could. That is why the previous cut had to be so close to perfect. this tool only shaved 5 thou at a time. New ones are only $200+


----------



## Karl_T (Feb 29, 2016)

Here's the charge handle slot being cut. Goes so nice'n'easy with all the chain drilling doen ahead of time. I meant to take a pic earlier in this tool's op. You can just barely see the top outline of the receiver is completely cut in some places and only cut to half depth in others. this keeps the part from falling out of the soft jaws.




OK, the CNC work is done. Here, the part cut through areas are finished off with a band saw. The 1/2 depth slot makes a perfect guide to saw by.


----------



## Karl_T (Feb 29, 2016)

Plan A was to manually mill finish the top outline. Turns out its easier to just grind and file.Plus there are several square corners




The proof is in the pudding, The part fits the weapon perfectly. Just so you know I ain't that good, part 1 (shown) was off 10 thou is several spots. Would have been "good enough" if I just wanted a shooter.


----------



## Karl_T (Mar 11, 2016)

OK, couple notes on the production run of five plates...

First, I love the Sandvick R390 inserts for rapid metal removal. But the chips come off blue hot and make a mess in the shop. So, I built this chip pan.

Not shown, I lay a USPS flat rate box top over the pan when running. Keeps 99% of the chips inside.





Also, had real trouble with part finish. The whole part was too thin and flexing away from the cutter, leaving chatter marks. So I build a support bar that couple be raised in place on a couple 1/2 x 13 bolts. For the heavy cut, put a piece of 1/8 rubber on top the support bar and just snug it up against the part. I scrapped a part making this too tight, it pushed it right out of the soft jaws and the part was too thin.


----------



## Karl_T (Mar 11, 2016)

OK, next op is cutting the top edges to correct height and thinning the top cover area from 0.187 to 0.125 thick

First job is build a good fixture, the key to machining anything. This is just a 5"x 15" x 3/4 bar and a 2" x 12" x 1/2" plate with holes drilled to go through the receiver charge handle and just in front of the ammo slot. Clamp the large bar in the vice. the top edge of the vice locates the bottom of the part for height.



I used "Manual NC" here. that is record your machine steps and do the same thing five times. I'm keeping this fixture for the future and recording my machine notes here. I always print out the instructions and tape to the fixture.




1. Set Z(knee) Zero at 3.588 overall height of RSP.
2. set X0 at front edge of ammo slot cut,  1/2" cutter to left.
3. set Y0 on front side of RSP, cutter to front
4.Machine top to knee 0   3.588 height
5. set Z level  down 0.213- on knee to 3.375 height
6. machine top  from x0 to x4.30
7.set Z level down to 0.388- on knee to 3.200 height
8. Machine from X0 to X 3.2 on front edge from Y0 to Y0.062, part thickness 0.125"


----------

