Cancel
Showing results for 
Search instead for 
Did you mean: 

Operation Navigator benefits

Siemens Valued Contributor Siemens Valued Contributor
Siemens Valued Contributor

Overview

This Tech Tip illustrates several key features of the Operation Navigator and shows how to make the best use of this powerful feature.

 

33.jpg

 

This Tech Tip was created with NX 8.5

 

Details

The Operation Navigator is the utility in NX CAM used to create, modify and manage your NC operations.

The utility offers a very effective way to manage the NC operation in 4 different views, such that it becomes easy for the programmer to categorize the operations, the tools used, tolerance settings etc.

 

The four views are:

  • Program Order View
  • Tool Order View
  • Geometry View
  • Method View

An advantage of the 4 views is the inter-linking of the views, such that the operations or objects created under each different view can share the information stored where needed, which helps in effective way of programming and reducing the programming effort.

 

Geometry View

 

This is the view where we create our geometry types like MCS, WORKPIECE - Parts/Blank and Check Geometries, Cut Area, and Boundary Geometries etc.

Objects created here, or for that matter in any viewing group, follow the parent and child relationship, as indicated by the level of indent. Any child (more indented) object will inherit the properties applied in parent (less indented) object.

 

28.jpg

 

As seen in the image above, MCS_MILL is the object at the top level in the navigator tree and the WORKPIECE object is created as a child object the below the MCS_MILL, and so on for MILL_AREA and the operation.

 

So going up from NC operation level, the operation (i.e. ZLEVEL_5AXIS_1) is inheriting the area to be machined from its parent MILL_AREA, which further is inheriting the Part and Blank geometries from the WORKPIECE object.  And finally, all of these are inheriting the Offset value from the MCS_MILL.

 

Any tool path operation created under the MILL_AREA, will be inheriting the values specified in all the parent groups above it in the navigator tree.  This reduces the effort in programming by enabling us to define MCS and Geometries only once and any number of tool paths created will automatically know the inputs from inheritance properties.

 

Also NX offers the flexibility to move an operation from one Geometry group to another, just by drag & drop functionality.  When an operation is moved to a new geometry parent, it changes its inheritance values automatically. As we see in above image the Drilling operation is created under the WORKPIECE object, so it will not inherit the Cut Area, which could be different for this drilling operation, but it will still inherit the Part Geometries and MCS Offset values which need to be same.

 

With this functionality, NX offers a very easy way to avoid duplicating the effort of specifying the same parameters again and again. It is also a very flexible way to manage operations in different geometry groups for different inheritance requirements.

 

 

Machining Method View

 

In Method view the user can categorize the operations depending on the machining method like Roughing, Semi-Finishing, Finishing etc.  Of course, users may create as many different Methods as needed to conveniently provide inherited parameters for their particular machining process steps.

 

There are several cutting parameters that tend to be distinct for these different Methods, so specifying them once as a Method parent allows several operations to inherit these parameters in the same way that Geometry specifications are inherited. Parameters that can be inherited from a parent Method include: part stock, tolerances, feeds, etc.

 

29.jpg

 

As seen in the image above the ZLEVEL_5AXIS_1 operation is placed under MILL_FINISH method, so the operation will inherit the values specified in the parent group, and so on for any additional child operations under this parent Method.

 

In this case, parameters like Stock, Intol/Outtol, and Feeds will be transferred to the operations placed under any specific Method group. As seen in image below.

 

30.jpg

 

 

Machine Tool View

 

Same function of Inheritance and parent child relation is applied in the Machine Tool view; here users can manage the tools used for groups of operations. Any number of operations created with the same tool can be arranged and seen under the same tool parent in the navigator tree.

 

As seen in the image below, both the Z-level operations are using same tool and hence are placed under the same tool parent. Also here the operation will inherit the properties of ‘Tool Number, Tool Length Register and Cut-com Register’, from the Pocket_01, based on inheritance principle.

 

31.jpg

 

 

Program Order View

 

The Program Order view shows the sequence of the operations as they will actually run on machine tool. This sequence also is the key to calculating the level based In-process Work-piece (IPW) results for any operations that follow a level-based IPW operation within that group.

 

Besides just specifying the actual cut order, another advantage of the Program Order view is that users can create and manage the NC operation in the groups as suited to the specific job.

 

As an example if the job needs to be machined in 2 different setups and the user needs to manage the operations for both setups, we can create Setup_1 and Setup_2 Program Group parents and locate the NC operations inside the respective Program Groups.

 

This approach helps manageme several operations and avoids any confusion.

 

Interlinking the views

 

We have gone through the individual advantage and usage of different views of operation navigator. Now let’s go through some advantages of inter-linking of these views.

 

One advantage of these groups is that the NC operation placed and located while creating new operation, under the required fields considerably reduces the program time and effort as all the important required parameter are fulfilled, i.e. the Tool is inherited from Tool and Pocket objects in Tool View, Geometry is inherited from Geometry groups in the Geometry View, and Stock, Tolerance and Feed are inherited from the Methods in the Method View. Once the parameters in these groups are correctly defined, the only major job for the programmer is to just Generate the operation.

 

See the image below - the Location block lets you select all of these parents as you wish, right when you create a new operation.  

 

 32.jpg

 

Another major advantage is the automatic set up of cutting data, which is based on Tool Material, Part Material, and Method (like Roughing, Semi-Finishing or Finishing), and these values are inherited by the operation simply by locating the operation under required Groups in different views.

 

User Interface of Operation Navigator

 

NX displays some very important information needed while programming right in the Operation Navigator. This information can be accessed and seen up front, without opening the individual operation dialogs, as seen in the image below. We can see the Tool used, Path Status, Time, Method used.

33.jpg

 

User can customize the information columns by right mouse button click in empty space in the Operation Navigator. Choose Columns, and check or un-check options as you choose to make the up-front information environment more suitable to your needs. As seen in the image below.

 

34.jpg

 

the Dependencies tab at bottom of the Operation Navigator shows the dependent objects, both parents and children, of the selected item in the main Navigator section.

 

35.jpg
 

 

Do you have a question?

Click 'Add a Comment' below to ask it. (You must be signed in to access this feature.)

 

About the Author

 

Lars Lars Okkels is in the Manufacturing Business Group at Siemens PLM Software and focuses on part manufacturing solutions especially for Mold & Die. He has been in the industry for over 15 years and enjoys supporting NX users applying innovative manufacturing technology solutions. Lars is originally from Denmark and now resides in Shanghai, China, with his family.

 

Best regards

Lars Okkels
Siemens, MBG
Comments
Pioneer
Pioneer

Hi All,

 

Thanks for the information. 

I am customising the information columns using NX-Open and have the following issue.

 

Problem:

When the session closes, the information columns are reset.

I would like to retain the information so that I don't have to customise manually every time.


Question:

Does NX store the column inormation in any file/egistry?

If yes, Where can I find the file which NX uses at launch to set default columns.

 

Thanks.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

The ONT columns are saved in the users registry, therefore they are hard to apply to multiple users.

There is an enhancement request to store the column customization in a way that is better to deploy to multiple users and to configure.

Pioneer
Pioneer

Hi Stefan

 

I have also raised an enhancement request for the same.

Thanks for your time and response.

LIVE Tech Tip Webinars
Watch NX experts demonstrate manufacturing best practices. Stay online for Q&A.