1. "It seems pretty straight forward so why doesn't that toolpath work for this?"
It all depends on your settings in Floor & Wall. The likely settings that may be preventing the desired tool path are under the Containment tab of the Cutting Parameters. Play with those settings one at a time and see what the output looks like to understand what each of them do.
That being said, Rest Milling is usually better for this situation because it is designed for such things. Picking out stock in tight areas where the previous tool couldn't fit accroding to the IPW is what Rest Milling is made for.
2. "Second question, why didn't the .250" EM in the last Rest Machining toolpath go down into the .500", .4375" and .375" holes that are all over this part?"
Honestly, this question is a little bit odd. Most users don't want the roughing operations to go into such holes because they plan on creating hole making operations on those features later in the workflow, usually after the milling is done.
However, if this is what you desire then this probably can be done. You will need to change some default parameter settings to get this. Look into the Non Cutting Moves dialog under the Engage tab. There, under the Closed Area group, you will see the Minimum Ramp Length and Minimum Clearance parameters.Change these numbers and see what the output is. They may be what's preventing you from cutting inside the holes.
Also, be sure to look into the Cutting Parameters dialog under the Containment tab. There is a parameter named Small Closed Areas. If this is set to Ignore then it will block the cutter out of the holes.
3. "What do I have to do to get rid of the toolpath segments on the corner of the Workpiece in the last toolpath?"
There are a couple of things you can do here. One option is to specify trim boundaries on the outside edges of the part and set the Side Trimmed to Outside. Another easier option is to modify the cut levels. Go into the Cut Levels dialog of the Rest Milling operation and expand the List group to see all the ranges of critical depths. Select the bottom most range and then select the bottom most part face that you want to cut. The bottom range will adjust to your selection and then the tool path will not go below it.
OK, I'll play around with all of the stuff you mentioned.
No, I am happy with the cutter staying out of the holes, sooooooo not an odd question at all. I was just expecting it to try and machine them is all. PowerMILL would try and machine them by default with multiple ways of preventing it from happening. It sounds like NX is just the opposite where it won't machine them by default untill you force it to.
Thanks for all of your input guys!
Also, it's strage that the Rest Milling toolpath has the levels based IPW and 3D IPW option but Floor Wall only has the 3D IPW option.
Rest milling is a special setup cavity milling operation, floor/wall is a volume 2.5d operation, which is a totally different an much more modern type of operation than cavity milling.
You can check this by selecting information from the context menu of the operations in the operation navigator.
---------- Operation Information ---------- Operation Name FLOOR_WALL Operation Type Volume Based 2.5D Milling ---------- Operation Information ---------- Operation Name REST_MILLING Operation Type Cavity Milling
Welcome to the NX wonderland
Production: NX10.0.3, VERICUT 8.2, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0
Employees of the customers, together we are strong
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide