Gunsmithing Ejection ports

[LRI]

Inletting a stock for a Bighorn action this morning. (That'd be you Mr. Corey!)

Never done one of AJ's actions for a full build before (least I can't recall doing one) and since ejection ports are kind of cool to inlet (surfacing) I took some pics.

Pretty simple in regards to surfacing. You just draw the general outline, copy and paste it a 3/4 inch in the +Y direction and generate a lofted surface from the two features. Stitch it together for the tool containment and your done with the drawing stuff.

Next you assign a tool path, select your tool, feed/speeds/stepover and filter the snot out of it so that its posting the radius moves as arcs instead of splines. (Splines are short line segments that make a machine behave like it has Parkinson's disease) Arc movements are much smoother.

This however requires playing with the work planes. Thankfully the newer software does this for you when it posts. Older versions required you to go in and edit post processors. (which is a lot like playing roulette with a loaded single shot)

Editing post processors is not a task for the weak minded. (which explains why I suck at it) One wrong +/- and suddenly your machine tries to friction weld the spindle into something.

PICS!

 

[LRI]

Re: Ejection ports

Fitted. Onto the bolt handle inlet. Then were ready to flip it and do the bottom side.

 

[LWILLIAMS]

Re: Ejection ports

You make that look to easy as always.

 

[Skyking]

Re: Ejection ports

Nice work Chad. Seeing these post is why I decided to give you try in the first place. It's nice to see your own gun being built. Keep up the good work.

 

[jrm850]

Re: Ejection ports

I appreciate you posting the code. I didn't have a cnc when I was building guns so I have a few questions if you don't mind sharing your knowlege.
I noticed your plunge rate was at 5ipm. Is this to prevent chipout?
Is a climbing cut cleaner on the edges than conventional?
Are the green lines your toolpaths in the image above? It looks like a tight stepover.

Lofting the polylines looks like a really nice and quick feature. To do the same thing in my setup, I would have to make a positive in Solidworks and export to CAM as an stl for surfacing. Is that feature in your CAM or directly in your controller?

 

[LRI]

Re: Ejection ports

<div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: jrm850</div><div class="ubbcode-body">I appreciate you posting the code. I didn't have a cnc when I was building guns so I have a few questions if you don't mind sharing your knowlege.
I noticed your plunge rate was at 5ipm. Is this to prevent chipout?
Is a climbing cut cleaner on the edges than conventional?
Are the green lines your toolpaths in the image above? It looks like a tight stepover.

Lofting the polylines looks like a really nice and quick feature. To do the same thing in my setup, I would have to make a positive in Solidworks and export to CAM as an stl for surfacing. Is that feature in your CAM or directly in your controller?
</div></div>

First, ROCK ON! I love questions like this!

The surface is lofted. Simple and quick to generate and very stable when farting around with them.

5ipm is as you suspected, to mitigate blasting through the bedding/stock material and tearing out a big ol chunk. One thing I always try to be conscious of is spindle speed and cutter diameter, especially with ball end mills. I have to use a cutter with a radius smaller than the corner fillet. If I go bigger then the surface won't be accurate cause the radius of the cutter is too big.

Small cutters demand a high spindle speed in order to generate the surface speed required for them to machine properly. I only have so much on the ol Haas so being conservative with the feedrates is a must. Plus it gives me the opportunity to hit "big red" if something looks goofy. That's always a plus. If I were running a hundred of the same stock I'd take the time to modify my entry point so that it wasn't a straight Z move into material. I can goof with start/end points in the software buts just more time consuming. Each one of these inlet features gets written individually so time is precious.

I run a parallel surface toolpath. Quick/dirty/simple/stable and very code busy. Especially with a .005" stepover. I used to run them at .02" but then it ended up with me having to sand the scallops out by hand. Faster to just do it once in the machine.

My software will allow me to generate geometry and post code in one package. Simple stuff like this I just do it and roll. For more complex parts (like my scratch built 80cc twin cylinder nitromethane breathing reed valve 2S giant scale pylon RC plane engine I did the design work in Autodesk Inventor. CAM packages just aren't as user friendly when working with solids.

 

[RugerSlinger]

Re: Ejection ports

<div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: C. Dixon</div><div class="ubbcode-body"><div class="ubbcode-block"><div class="ubbcode-header">Originally Posted By: jrm850</div><div class="ubbcode-body">I appreciate you posting the code. I didn't have a cnc when I was building guns so I have a few questions if you don't mind sharing your knowlege.
I noticed your plunge rate was at 5ipm. Is this to prevent chipout?
Is a climbing cut cleaner on the edges than conventional?
Are the green lines your toolpaths in the image above? It looks like a tight stepover.

Lofting the polylines looks like a really nice and quick feature. To do the same thing in my setup, I would have to make a positive in Solidworks and export to CAM as an stl for surfacing. Is that feature in your CAM or directly in your controller?
</div></div>

First, ROCK ON! I love questions like this!

The surface is lofted. Simple and quick to generate and very stable when farting around with them.

5ipm is as you suspected, to mitigate blasting through the bedding/stock material and tearing out a big ol chunk. One thing I always try to be conscious of is spindle speed and cutter diameter, especially with ball end mills. I have to use a cutter with a radius smaller than the corner fillet. If I go bigger then the surface won't be accurate cause the radius of the cutter is too big.

Small cutters demand a high spindle speed in order to generate the surface speed required for them to machine properly. I only have so much on the ol Haas so being conservative with the feedrates is a must. Plus it gives me the opportunity to hit "big red" if something looks goofy. That's always a plus. If I were running a hundred of the same stock I'd take the time to modify my entry point so that it wasn't a straight Z move into material. I can goof with start/end points in the software buts just more time consuming. Each one of these inlet features gets written individually so time is precious.

I run a parallel surface toolpath. Quick/dirty/simple/stable and very code busy. Especially with a .005" stepover. I used to run them at .02" but then it ended up with me having to sand the scallops out by hand. Faster to just do it once in the machine.

My software will allow me to generate geometry and post code in one package. Simple stuff like this I just do it and roll. For more complex parts (like my scratch built 80cc twin cylinder nitromethane breathing reed valve 2S giant scale pylon RC plane engine I did the design work in Autodesk Inventor. CAM packages just aren't as user friendly when working with solids.

</div></div>

More info please, I love this shit!

 

[jrm850]

Re: Ejection ports

Awesome engine! Is that trochoidal milling in the last pic where you are roughing the cylinders or just a bigger stepover? Are you making your own rings for it?
I had the RC heli bug for a while but they are just ground magnets. I could fly the heck out of them on the simulators, but ended up choking on a regular basis is real life. I think I'm going to sell that stuff on ebay so I can put the cash towards some blanks or optics.

I put a 30k rpm auxilliary spindle on my little Tormach for routing PC boards, but it works pretty well for finishing passes when 3d profiling. Aluminum and plastic is all I have tried it on so far. My main spindle is limited to 5100rpm so it's a pretty slow process to profile with small diameter cutters. I've only had the cnc for a couple of months now so there is still a lot to learn. 20+ years on a manual helps somewhat, but putting actual numbers on feeds and speeds takes a little getting used to. Sometimes I just put my hand on the mill bed to see if it feels right.

I've been using G-Wizard for base numbers and tweaking from there. I can't believe I waited this long to get one though... I'm completely hooked. The last project that was underway when I quit smithing was a little .22 hornet double rifle. I still keep the unfinished project in my office as a monument of some sort. If I would have had this mill then I could have knocked it out in short order. An interesting side note about that project related to cnc is that I ordered some super thin barrels for it from Walther (.408" at the muzzle) They asked if I wanted them to pre-chamber and I told them that I was going to spec my own reamer. They said no problem because they cnc'd the chambers anyway. I have always been intrigued by that thought. Any caliber, any spec, any time. I have no idea what they used for a boring bar that small that wouldn't chatter like crazy but as soon as I get a cnc lathe I'll be trying it.

Anyway, I enjoy your build posts and trying to learn a bit from your code.

Jeff

 

[Millsaps75]

Re: Ejection ports

Hey Chad are using mastercam X? Its pretty darn good software.I'm actually a little more accustom to mastercam 9 but X has some nice featurers. I inlay all my stocks on my matsuura vmc. I usually do the action port on the Bridgeport by side milling but I think you've inspired me to draw up a surface and 3d cut in next time. Great job on the rc case. I wish I had more time to do stuff like that. Got love 3D machining.