I have been teaching custom model features to the MKE with reasonable success, but I wish to now point these features directly to templates I have created in the mach\template_part folder.
Is this possible using the MKE?
It looks like we can define operations and specify tooling etc as the MKE is intended, but maybe I'm looking for something a bit different?
The reason I want to do this is to point to a template file that is basically a call for a sub program which will machine the custom feature - as opposed to creating a new NX program through the machining rules.
These sub programs are "Best Practice" approved and released for production. We could not sustain having to verify all new programs - our parts are on machines for days.
Thanks in advance.
Solved! Go to Solution.
We have introduced a new capability in NX12.0.1 that we call "Operation Set Based" FBM. You can find a brief introduction in the NX12.0.1 What's new guide.
This allows you to use Teach Operation Sets from inside NX (which creates a sequence of machines rules for you in the MKE). But instead of then using Create Feature Process -> Rule Based, you use Create Feature Process -> Operation Set Based. This workflow will allow you to select one or more features and ask the user to select the sequence of operations that you want to use.
So there is less automation and the user can select from alternative sets of operations.
You can make this as intelligent as you want. Either it's really specific; e.g. you select the process for an M6 hole; it contains the exact operations and tools and you make sure (by putting an application condition) that the sequence can ONLY be used for an M6 hole OR you allow the process to be used for a range of threaded holes (e.g. M6 - M12) and you add tool selection conditions.
So this is very much like the Insert -> Geometry Object from template (with the child operations) but with:
- Automatic check on feature types to filter and show only operation sets that work on the selected feature type
- Optional application conditions to check if the selected sequence of operations can be applied to the selected feature instance (e.g. checking the dimension)
- Optional tool selection conditions to select different tool size for different feature sizes
NX CAM Development
Tom van 't Erve
This is something I will revisit in the future but unfortunately we are still aligned on NX8.5 here and we will only change to NX11 later in the year.
I am still unsure of how to automate and connect our Standard Features to an agreed CNC program already released for Production, not creating a new one.
I have taught my standard feature, BX169 for example.
And I already have a CAM template that is simply a call for the necessary CNC sub program to machine this feature...
Yet, I'm unsure how to automate tieing these together. Tieing the feature to the template.
I thought the MKE would be able to simply link the feature recognition name, BX169, to a file location on the CAM drive that has the template called BX169 - this calls the CNC program that is necessary to machine this profile.
It would be nice and neat to do this function in the MKE as opposed to having to try and code the link in NXOpen.
If anyone has any input into a solution it would be appreciated.
This should be possible with classic MKE / FBM and fairly easy.
1. Add you templates like Heller-Sub_Prog to your template set file ( the .opt file ) if you had not already.
2. One time only use MKE "Open and Update" to get your operations into the customization.
3. Create the machining rules in the MKE, for instance for a BX-169. Since NX does not accept a MILL_CONTROL operation directly under a Feature Group, you must create an Add-on of type GeometryParent in between, as shown here:
4. Create Feature Process will give results like this:
Hope this helps.
I am having problems with the Geometries on this issue.
I have followed your steps above but when I Create Feature Process I get the following error.
If I manually add a new MCS under the WORKPIECE geometry, anywhere on the part then this "Create Feature Process" now works okay.
However, this should not be a step I have to take, as per your example. When the feature is found using "Find Features" the feature geometry is already defined. Should this not be picked up?
Can you assist further?
If you select the geometry parent the feature process will be created as a direct child of the parent.
You need to select the correct MCS below the WORKPIECE or use automatic selection.
The tool axis specified in the MCS group must match the Z-direction of the machining feature.
Production: NX10.0.3, VERICUT 8.1, 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
If you change the Tool Axis of the MCS_MILL to "All Axes" then the operation will be allocated below.
You can remove the MCS directly under Workpiece.