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How-to create a reference in draft from the assembly

Charles-Etienne Lavoie - Tuesday, August 12, 2014

How-to create a reference view in draft and keeping associativity to your assembly.

 

1) Place the assembly has you would normally do in a MASTER MODEL draft,

 

 

 

2) To create the individual views, return to the MODELING environment.

 

 

 

3) Open the exploded view menu




4) Orient the view to the desire position and save as

 

 

 

 

5) From the exploded view menu, select hide component to hide the unwanted part




6) Hide the component

 

 

 

7) You can use the show component in view to show component

 

 

 

 


8) Save the work view when done

 

 

 

9) To change the work view to a canned view, RMB in the work environment and select replace view, from there select any view or use custom for a more specific view.

 

 

 

10) Return back to the drafting environment and add the newly create view to your sheet

 

 

 

 

 

 

How to create an adjustable coil spring

John Pearson - Wednesday, September 18, 2013
How to create an adjustable coil spring

If you wish to create an adjustable part, you must build a part that is adjustable. Sounds obvious, but sometimes what seems adjustable to the eye is not adjustable in the CAD system. For example, let’s look at this coiled spring.


New users may look at the part and model it using the helical protrusion command to make the coil. Then use protrusion and/or swept protrusion to complete the part. This will look good but will not be adjustable. Why? Let’s look at the part in an adjusted or deformed state.


Notice that the coil deforms as the part adjusts. If you model this with a helical protrusion, the rules of the helix will prevent you from deforming the coil. So how do you model this to get the adjustable results?

There may be other ways to model this part, but I find this method fairly easy to create while giving me the control I need. I start by creating a flat sketch of my part, on the Top reference plane.



Notice the 2 lines labeled A. These lines represent my wrapped coil center lines. My wire will be 7.5 mm in diameter, so I’ve made the opposite ends 8 mm wider, to avoid any body intersection. The 157.1 mm length of these lines is equal to the perimeter of the initial coil size. I‘ve used two tangential arcs to create the lines, because it generates a nice smooth flowing coil.

I then create a second sketch on the Right reference plane to represent the initial coil position.


The top quadrant is connected to the (0,0,0) point with the center of the circle horizontally aligned beneath it.

I then create an extruded surface, which I will use to wrap the coil around. The Extruded Surface command is found on the Surfacing Tab, in the Sufaces group.



Next, I use the Wrap Sketch command to wrap the arcs around the extruded surface. This command is found under the Surfacing tab, in the Curves group.



I am first prompted to select the face that you will wrap around. I select and accept the extruded surface.





I am then prompted to select the sketch that I wish to wrap. I set the selection filter to single and pick the four arcs from the sketch.



Once I accept the selection, the arcs wrap around the extruded surface.




To make it easier to visualize the next steps, I hide the extruded surface. I then create a sketch, to represent the diameter of my wire, centered on the top of the flat wire, on the Front reference plane.



I then use the Swept protrusion command to create 3 features. Note: I use the following options when creating all 3 features.




The first swept feature looks like this:



The second swept feature looks like this:


The third swept feature looks like this:





Finally, I hide all sketches and curves, and then I create the last two wire sections. I could use several different methods to create these sections, but for simplicity I used the Thicken command, and simply thicken the end faces the distance that I need.


I now have the modeled part which I can make adjustable.

In this model we want to adjust the tilt angle of the legs, which is actually controlled by adjusting the diameter of the coil.

To simplify the process I open the Variable Table and rename the variable that controls the diameter of the coil, to Coil_diam.



I then create an associative sketch, on the Right reference plane, to allow me an easy way to monitor the tilt angle of the legs.



Note: I used the Include command to create this associative line.
In the Variable table, I located  the 90 degree variable and renamed it to Tilt_angle.



If I change the Coil_Diam  value, I will notice that the Tilt_angle  value changes because of the associativity between the Sketch and the model.

For example, if I change the Coil_Diam to 55 mm the Tilt_angle changes to 57.27 degrees.




Now that I have this relationship, I can use the Goal Seek command to get the exact Tilt_angle  value, that I need. 

I select the Goal Seek command from the Evaluate group, under the Inspect tab.



On the command bar I input the following information;


Goal: Tilt_angle
Target: My desired Tilt_angle (e.g. 45 degrees)
Variable: Coil_diam





When I accept this input, the Goal Seek will run through a series of iterations, until it finds the exact Coil_Diam value, to give me the desired Tilt_angle value. 

In the example, the results are as follows:



I now have a part that can easily be adjusted, without having to create any complicated formulas.

Note:  Clearly the deformation of the coil has it limits. If you enter in too large of a Tilt_angle, the model may fail. I have also kept this example simple; therefore if you try too many different angles, without resetting back to the original angle, the model may fail.

It is important to note that this example could be created in several different ways and still provide you with similar results. The main thing here is that the model must have the flexibility to adjust. If I had used the Helix command instead of the Wrap Sketch command, I would not be able to adjust the coil. I can also obtain the desired results using the Goal Seek command. This saves me from having to derive complicated mathematical formulas. 




NX – Create a family of standard parts (Excel)

Charles-Etienne Lavoie - Wednesday, July 04, 2012

                   

                  Design Intent:


                  The most common use of Part Families is to define a standard library part that has many variations.


                  1. Create a hexbolt 

                   


                   

                  2. Rename the expression that you want to keep


                  •   a-Width = the radius of the cap

                    b-Length = length of screw

                  •  

                  3. Define the columns for the Family Table.

                   

                    Choose Tools→Part Families from the main menu bar.

                    Make sure the Importable Part Family Template option is cleared.

                    Click OK on the Warning dialog box.

                    Select the width expression from the top window of the Part Families dialog box.

                    Click the Add Column button.

                   



                    Select the length expression from the top window of the Part Families dialog box.

                    Click the Add Column button.


                  Note:

                  Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.

                   

                    Change the option menu at the top of the dialog box from Expressions to Features.

                    Double-click chamfer from the top list of the Part Families dialog box.


                  Note:

                  The order in which you select the attributes determines the order of columns in the spreadsheet.


                  Tip:

                  In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.


                  4.Create the family table.

                   

                  •   Click the Create button from the bottom portion of the Part Families dialog box.

                   


                   

                  •   Type in a few values



                  5.Verify a family member

                   

                    Select a cell in row 3.

                    From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.

                   


                   

                  The NX session becomes active and the family member is displayed in the graphics window.

                    Click Resume in the Part Families dialog box.


                  Warning:

                  The Part Families dialog box may be obscured, if so, click anywhere in the NX window.


                  6.Save the Part Family and the template part.

                    From the spreadsheet menu bar, choose PartFamily→Save Family.


                  Note:

                  The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.


                  Note:

                  In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.

                   

                  Since we do not use this part anywhere else we are not going to do that.


                  7.Close all parts.

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



A new look pattern command in NX8

Charles-Etienne Lavoie - Monday, March 05, 2012

With NX8, the pattern command got a fresh new look and more command features associated with it.

One of the new features is the simplified boundary fill; this feature will fill the specified face with three different pattern layouts;

1- Triangle

2- Square

3- Diamond

This can easily be done in a single pattern, so no more having to position the origin of the feature, just select the feature, select the boundary face and voila!