Plunge normal refers to entering a cut in the vertical direction.
This is is one of the simplest and more affordable CAM software that you can start using for free http://www.estlcam.com/
Goto Google searching for “Fusion360” and “CAM”. You will find very good informations. So I learned the Fusion-CAM 
Paul Shaws postings are very good for learning!
@Paul_Shaw I can’t find my machine in post processing. I find emc but when I try the gcode i get an error code
Status update! I made some cuts! Found out that some gcode lines are messing with my controller. Need a fix for that. And for some reason the machine is plunging 1mm when I have it set to only go .5mm. I think there’s an issue with the gcode not understanding that I’m cutting a 7mm part out of a 9.525mm piece of aluminum
There is an online community here: https://groups.yahoo.com/neo/groups/sherlinecnc/info
This is the overall process I use with my Sherline mill for making parts:
http://www.davehylands.com/Machinist/CNC/Making-A-Part/
With a mill, the normal convention is that Z=0 is the top of the material that you’re going to machine. Negative Z coordinates cut into the material and positive coordinates are above the material (but you still typically need to take clamps into consideration). I also set things up so that the XY origin is in the bottom left corner, and my X and Y coordinates in the gcode are typically all positive.
I’ve only ever done 2.5D machining and not ever done 3D. I use either SheetCAM or CAMBAM to generate my g-code.
Near the end of this blog post: http://blog.davehylands.com/2015/04/ox-build-part-6-spindle-and-first-cut.html
I figured out how to pick off geometry in CAMBAM from an imported STL file.
The process of generating the gcode for machining is definitely different from 3D printing. You really need to think about the operations that you’re going to perform (drilling holes, pocketing, profiling, etc) and the order that you’re going to do these in. For normal parts I normally go in the order: spot drill, drill, pocket and profile. I also try to group operations to minimize the number of tool changes.
I’ve been using OpenSCAM from http://camotics.org to do my gcode simulations. It’s free and runs well under Linux (which is now my OS of choice). Its a bit quirky, but otherwise seems to do a reasonable job.
You need to get the z zero correct. In the 360 cam set up what have you got as you origin is it a model or stock point? How is your stock defined relative to the model?
@Paul_Shaw ya I just figured that out so I’m finally cutting. I’m able to spit out gcode but I need to delete the first 10 lines first. My last concern is if it’s going to cut through all the material material or too far
@Paul_Shaw nvm just figured out that setting. I guess my only issue now is to where I dont need to manually edit code
@Derek_Schuetz you need to do some calibration tests, to insure the steps per inch are correct for the software that is running your machine. I am confident you can find some YouTube’s on this. What is the name of the software that runs the sherline mill?
@Bruce_Lunde Linux emc. I’m pretty sure my steps are good it’s just was just me and still is me learning the software
Yeah I manually cut out the g53 z0 move that 360 puts in as it can cause issues for my machine. Is that what your problem is?
@Paul_Shaw ya those are the ones. What are some good speeds to cut aluminum at. I think I’m going to fast now. Currently doing 100mm/min and .5mm depth cuts
I normally do 3-5 IPM (wihch is 75-125 mm/min) for finishing and 10 IPM (or 250 IPM) for roughing (with a 1/4" or 3/8" endmill). I typically do 0.020" depth of cut (0.5mm) for roughing and half or quarter that for finishing.
That’s for 6061 or 7075. Pure aluminum is gastly stuff - very gummy - so I avoid it. This is what you often get when you buy aluminum stuff at your home hardware store. I normally use 2 flute endmills, and use very small amounts of tapping fluid (or cutting fluid).
@dhylands so my cutting speed and depths seem good. So I think my issue is just setting up a part. I’m cutting into one giant sheet of aluminum jist doing small sections what appears to be happening is the Cnc thinks there nothing on the edges and will come into the cut cause I’m assuming skipped steps
Yeah if you’re doing a full width of the endmill cut, then you probably need to slow down a bit more. I normally cut my pieces roughly to size using my bandsaw and then do the finishing on the mill.
Plunging is bad since the cutting speed near the center of the endmill is really slow, so I normally drill a hole slightly smaller than the endmill and then plunge the endmill into the hole. Then the cutting happens near the edges where the speeds are more appropriate.
If you do need to cut into a sold piece, then you probably want a ramp rather than a plunge. Usually that’s an option at the CAM stage.
@dhylands thank you for the advice I’ll see if I can find a setting for that