Showing results for 
Search instead for 
Did you mean: 

GEOMETRY vs. MCS_MILL selection.




I’ve been using NX for a few months now, mainly walking through and regenerating existing programs for similar, but different parts.  Lots of planar milling and point to point drilling being used and I’m starting to get the impression that the other programmers here like the “old school” way of doing things.  “That’s the way we’ve always done it” or “the new toolpath doesn’t work for crap” or I am offered an old weird cumbersome time consuming workaround to get some newer functionality of NX to work simply because nobody else here has taken the time to figure it out.  I don’t want to get stuck following them and their mindset (I've been down this road before) so I’m kind of on my own trying to figure a lot of things out.  My boss is pretty open minded (although he's not really a CAM guy) and just seems to want good toolpaths so I seem to have the green light from him at least to come up with whatever I want.  Why waste my time learning an old inefficient way of doing things?


That being said, I’ve kind of got ahead of myself to some extent and am having a difficult time wrapping my head around a few things.  For starters, on some toolpaths you are able to select either your MCS_MILL or a WORKPIECE under the “geometry” drop down selection box.  This is completely foreign to me.  If you select WORKPIECE then at what point and where do you select your MCS_MILL?  And why are they combined in the first place?  Could someone please explain the workflow of this.




Re: GEOMETRY vs. MCS_MILL selection.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Generally the MCS is a parent of the workpiece.

All the NX CAM views (program order, machine tool, geometry, method) "inherit" settings from parents to children.


If you pick the MCS as the parent, that's all you get.

If you pick the workpiece (assuming it is a child of the MCS) you get the MCS, PLUS you get the part & blank (assuming they have been set in the workpiece)


You might benefit from some training.

You could try Learning Advantage (if you have access/license) or look in the tech tips area here, or (heaven forbid!!!) read the manuals.  Note (supposedly) for every dialog, if you hit the "F1" key, it will jump to the section of the docs that covers that dialog (context sensitive help).

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled

Re: GEOMETRY vs. MCS_MILL selection.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

You can have many ways to specify things:

      • MCS_PRESET_1
      • MCS_PRESET_2
      • etc.

You may call the MCS_PRESET also MCS_FIXTURE_OFFSET. which resembles the purpose inside of it.

We mostly have something similar to:

      • MCS_MILL_TOP

The difference is mostly, that for milling we delete ejector pin holes and similar that violate the shape of the molded part.

So selecting any child will also include the objects contained in the parents.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.2, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 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 Smiley Wink
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide

Re: GEOMETRY vs. MCS_MILL selection.


Since being trained in NX I always did the following structure


3 axis only




5 Axis

MCS MAIN (Placed at machine zero point)


>>MCS for rotation


But recently I talked to another user and for 5 axis have adapted the following strategy which is very helpful for doing 5 axis work where sometimes you need to make toolpaths not using the model as the part



>>Workpiece (only with Stock)

>>>Workpiece (with part)

>>>>MCS for rotation


This way when you verify it always knows where the stock is


Dennis Rathi
Creations Unlimited

Re: GEOMETRY vs. MCS_MILL selection.

Siemens Phenom Siemens Phenom
Siemens Phenom

Some operations may take a long time to calculate when looking at the entire solid, using the MCS and a workarea speeds up this process, but gouging is a posibilty...

Re: GEOMETRY vs. MCS_MILL selection.


So you're talking about just selecting faces from the solid for the area (or general area and then some) that you want to cut correct?  I understand how that helps calculation time but how does using the MCS help?

Re: GEOMETRY vs. MCS_MILL selection.


Anything under that MCS inherits the tool axis so you dont have to define it in every operation over and over.


Dennis Rathi
Creations Unlimited

Re: GEOMETRY vs. MCS_MILL selection.

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Welcome to the world of NX CAM.  Where there are multiple ways to do the same thing.  I encourage you to get some training, easy for me to say.  Learning advantage if good if you have access.  The help docs are avaialble.  There are a lot of videos on Youtube.  Unfortunatly you can also learn some bad habits. I will also encourage you to ask questions here.  This is a very helpful community.


The type of machine your going to program will sometimes dictate how you set things up in NX.  As others have already commented on.  Even for 3-axis work you may need to talor the Geometry to fit your needs.

For example - using multiple work offsets







The biggest hurdle, in my opinion, is the post -processor.  If this is not correct or does not take advantage of the available options in NX then you will have to find ways around that or get the post corrected.


And Yes there are times when the "Old School" way still works the best.


John Joyce, Manufacturing Engineer,
Senior Aerospace

NX Vericut 8.0.3 - Statements and opinions are mine alone and do not reflect
the opinion of my employer or any other member of the human race

Re: GEOMETRY vs. MCS_MILL selection.


To your original question... If you select WORKPIECE then at what point and where do you select your MCS_MILL?


If you did file--> new--> manufacturing, the template part set you up in this configuration




Putting your tool path under the workpiece "inherits" the MCS because of the parent/child relationship

* If I open the tool path, I can't pick a part... I already have a part "inherited" from the workpiece.




Now if I switch my geometry to the MCS... I have to pick a part in the process. One is not pre-selected from the workpiece.

** Note how the tool path is no longer branched off the workpiece




As a new guy and if the work is not terribly complicated your toolpaths will go under the workpiece for the most part, every set-up operation should be a new manufacturing part where you can get the IPW (In-Process workpiece) from the previous manufacturing file. It works great.


But... it is all drag and drop... so workpiece at the top and MCS as a child of it will give you the same results.


....Before the days of getting the IPW to go from Set-up to Set-up. Workpiece at the top was a good cheater method to carry an in-process part from operation to operation. Each MCS under the workpiece could have a different oriention (set-up) and the part you started with at the top would be carried thru all operations by the time you got to the end.




** in the program order view the tool paths would be in (2) seperate program groups Op1 and Op2


I highly recommend the class room training if you can get it. They will start you down the right path...



{Paul Schneider}, {CNC Programmer}, {DRT-Rochester}

Production: {NX11.0.2,MP5, NX12.0.2, MP4}

Re: GEOMETRY vs. MCS_MILL selection.


OK, so that part helps eliminate redundant mouse clicks, not calculation time.  Got it.

Learn online

Solution Information