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Designfusion Blog

Working With Revision Manager

Manny Marquez - Thursday, January 09, 2014

In the past few days, customers have called about revision manager and have asked several questions on how  they can move or copy assemblies to new locations.

There were a few main issues custumers have had in regards to Revision Manager, and what I have done is created multiple scenarios to tackle these issues .  

 

Scenario 1: Copy all assemly with all parts to new location.  

Scenario 2: Copy all parts associated to assembly and folder structure to new location folder.

Scenario 3: If a folder with parts related to an assembly gets nenamed  and links get broken, how to redifine links.  

 

Sample Folder structure (this can be any combination of folder locations) the point is that, we need to move or copy files to a new location.    

 

 

          Scenerio 1: copy all assembly with all parts to new location, this is ideal when you need to clone

          the whole asssembly to send to a customer.  

 

  1. 1. Open TOP level assembly with Revision Manager.

 

 
  1. 2. Expand then select all, this option makes sure that all files will be copied. Notice action is unchanaged.

 

3. Copy; this indicates the coping process.




4.The next step is to set the path for the new location to copy the whole assembly.

 

 

 

5. Final step is to perform actions. At this point the assembly is copied to the (new) folder location.
    However notice the subfolders are NOT copied.  This completes this scenerio.

 

 

   

          Scenerio 2:  Move the whole assembly with subfolder structure and related files only.

          Another method is just to copy all folders to the new location, but note that there may be

          files that do not relate to the assembly.

          In cases where you only need to move  files that relate to that top level assembly and keep the 

          same folder structure, files not related will not copy or move.  

 

6. Open selected assembly with revision manager.

 

 

 

7. We are going to move to (new location) and copy the same folder structure. By selecting the (rename)

    you are moving the files from the (original) folder.

 

 

 

8. Notice action is to rename document.

 

 

 

9. Now click on replace old folder (Original) with new folder (New). Then select replace all then cancel.

 

 

 

 

10.Once replaced, see new folder with new location.

 

 

 

11.Click on Yes and close Revision Manger.

 

12.Notice the new folder structure in new location, notice the subfolders are copied as well.

 

 

 

13.Review new folders using window explorer to take a look at the previous folder location; notice only

     files that were not associated to the assembly did not copy (This is also a good way to isolate

     assemblies) with the folder structure. This complete this scenerio.

 

 

          Scenario 3: Cases when a folder gets renamed and then you open the assembly and notice that

          all links are broken. This is very common in networks with many users.

 

14.So let’s go ahead and rename each folder as shown below, just by adding “1” at the end of each

     word.

 

 

 

     If you try to open the assembly now with RM or Solid Edge, the files will not open; you will get a notice

     that files are missing.

 

 

 

15.Click on the redefine links then select top level folder then ADD (make sure that the subfolder is

     unchecked).

 

 

 

16.The easiest way to get the folder address correctly is by going to the window explorer, and then copy      and paste.

     -(ManufacturedParts) is the original folder

     -(ManufacturedParts1) is renamed folder

     -click next twice

 

 

 

17. Click on Back twice  

 

 

 

18. Repeat for other folders

 

19.Next twice

 


    Close Revision Manager, and then reopen with top level assembly. This completes this scenario.

 

    This was also presented at one of our Solid Edge Productivity summits by Barry

    Shillingford.



NX – Modeling a tapered thread

Charles-Etienne Lavoie - Friday, May 04, 2012

Currently, the NX Thread command can be used to create a fully modeled straight thread. When
this command is run and the Detailed Thread type is selected a fully modeled thread will be
created. NX provides Modeling tools which allow users to create fully modeled tapered threads.
The Variational Sweep is one of these tools.

 

1. Create a Datum CSYS on the centerline of the thread at the start location of the tapered
thread.

 

2. Create the following expressions in the Expression editor.

 


 

ANGLE will be the included angle of the thread profile. This is typically 60 degrees.
L will be the length of the thread.
P is the thread Pitch which is the distance from thread to thread.
START_DIA is the diameter at the start end of the thread.
TAPER is the taper of the thread.
END_R will be the calculated value L*TAN(TAPER)+STRT_R.
STRT_R will be calculated as START_DIA/2.

 

All expressions should be created as Length type expressions except for the ANGLE
and TAPER variables. These two need to be set to the Angle expression type. If these
variables are not created as Angle type expressions they will not be selectable when
creating the feature.


3. Start the process by creating a Helix curve.

 



The Number of Turns will be calculated by dividing the Length by the Pitch or L/P using
the defined expressions. The Pitch variable will be specified using the expression P.


4. To create the tapered helix the Radius Method Use Law will be used. When selected
the Law Function window will be displayed. At this point select the Linear type.

 



5. Specify the Start and End radius values by supplying these expression variables.

 



Note that the tolerance of the helix can greatly influence the accuracy of the thread.
Initially the helix will be created to the model tolerance in effect when created. This can
be found at Preferences => Modeling => Distance Tolerance.


If the accuracy needs to be improved after the helix is created a higher tolerance can be
specified by editing the helix and changing the tolerance value.


6. After the helix is created select Insert => Sweep => Variational Sweep. Select the helix
curve as the path. For Plane Orientation pick the Through Axis option and select the
centerline of the helix for the vector. For the Sketch Orientation select the same axis.

 



7. When OK is pressed a Sketch will be created. At this point create the profile of the
thread. Constrain all geometry to the point that was created on the helix curve when the
Variational Sweep operation was started. This is an important step.

 



It is significant that the width of the thread be smaller than the Pitch (P-.01). If this width
value is too large then the model will intersect itself as it sweeps along the helix guide
curve. This would cause an invalid solid to be created.


8. When the sweep is complete a hollow thread profile will be created as seen below.

 



9. The thread would be completed by Uniting it to the model of the base of the thread.

 



This same procedure can be used to create a multi-lead thread. When creating the
Variable Sweep Sketch of the thread profile create two threads at half the Pitch in width.
See the sketch below along with the picture of the resultant multi-lead thread. The colors
of the different leads have been altered for emphasis.

 




Using tools provided in NX, users can quickly and easily model complex features.
Randall Waser