Hi all ,
I have been using NX10 for a about a year. I have updated to NX11 upon release. I still have a lot to learn. Is there a way to bulk edit stepovers for operations? or a way to bulk edit drive methods? i have a whole lot of toolpaths that i have copied and just need to change the step over. I have been changing them individually. Im sick of it. Any help would be great!
A journal should be able to help with changing stepovers, drive methods you probably have to do manually because you usually have to pick new things when you change the drive method like boundaries and surfaces.
There are sample journals located at C:\Program Files\Siemens\NX 9.0\UGOPEN\SampleNXOpenApplications\.NET\CAM, there are C++, Java journals also.
You can use the OntSelectionBoilerPlate file as a starting point. You may have to record a journal while changing the stepover to be able to see the variables used, then plug them into the boiler plate file. Use notepad to open the journal files.
Production: NX10.0.3.5, Vericut 8.1.4, ICAM V21
Development: VB.NET, Tcl/Tk
If the operations are all the same type, then a journal is the way to go. You could pick a hundred operations and set them all at once. As noted above, there are several samples to get you started. The best way to start is to record editing one operation - this will give you what you need. For example:
planarMillingBuilder1.BndStepover.StepoverType = NXOpen.CAM.StepoverBuilder.StepoverTypes.Constant planarMillingBuilder1.BndStepover.DistanceBuilder.Value = 34.56 planarMillingBuilder1.BndStepover.DistanceBuilder.Intent = NXOpen.CAM.ParamValueIntent.ToolDep
Note that it took 3 parameters in this case. Although stepover seems simple, it is actually one of the most complicated parameters. For example, there are 19 types in the system - tool flat, constant, scallop, number, passes, variable, multiple, .... And if you are setting constant, you need to say if the value is part units or %Tool.
So there is some effort to get a journal working for this, but if you do it a lot, you can reuse it over and over. In fact, you could have it prompt for the new stepover value, or maybe take the value in the first operation and copy to all the others. Lots of options.
Another option is a keystroke macro. This will work if all the operations have the same dialog - you would edit each operation, then run the macro. This may be good short term, but since this just records keystrokes, it will likely break in a future release when the dialog changes. A journal is much better because it sets the parameters, without regard to the UI.
That's great progress so far. For multiple selection, I would start with one of the samples for "OntSelection" and adapt it for your changes. The tech tip Learn to use Journal Files in NX CAM should get you started.
You would think some of this would be easier...
In my old CAM you could highlight a bunch of similar operations and default the shared parameters the same as the one you right clicked on....
Highlight all the Fixed Contour with area milling and right click the one with the correct stepover. Select "Overall stepover to :5%"
Why not use the feeds&speeds library to specify your technology values?
It can handle automatic setting of feed, speed, step-over and cut depth for you, whenever you change a tool, material or cut method.
This removes the need to mass edit operations entirely.
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