Archive for May, 2012

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Creating insert notches in sheet metal

Thursday, May 17th, 2012information

Recently I was asked if Solid Edge had a special command for making insert notches in sheet metal. These notches are used to insert tabs or pins in various assemblies. The image below shows a few examples of the type of notches I refer too.

 

To create these notches and others like them, I always use the Bead command in the Solid Edge sheet metal environment. Although designed to create beads, it also creates open ended beads, which are notches. To do this you start with a sketch which represents the length of the bead. For example, I may need a 6.35mm (1/4 “) wide notch, so I create a 6.35mm sketch line.

Using the bead command options, I select the overall shape of the notch. For example, I may need a U-shaped notch 6.35mm high and 10mm wide.

Notice that I set a lanced end condition. I could also use a punched end condition which allows me to extend the cutout portion of the notch.

If this is a feature that I will use often, I can save the settings for easy recall in the future.

Once I say OK to the options dialog, I simply select the direction that I wish to apply the notch.

The resulting bead feature can be edited by adjusting the options or editing the sketch. It can also be added to a feature library.

So my answer to the original question:  “Does Solid Edge have a special command for making notches in sheet metal?” is yes. It’s called the Bead Command.

guidelines

NX – Modeling a tapered thread

Friday, May 4th, 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.

Original article courtesy of Randall Waser, Siemens.