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Using Goal Seek to aid in model design

Thursday, July 19th, 2012content

The Goal Seek command is one of the calculation tools available for engineering problem solving. It is available in the 3D environments and while drawing 2D geometry in a 2D Model sheet, a drawing sheet, a profile, or a sketch.

The Goal Seek command automates engineering calculations, which can be based on dimensioned geometry, to achieve a specific design goal. Goal seeking finds a specific value for a dependent variable (dependent by formula, for example) by adjusting the value of another variable, until it returns the result you want. Goal seeking shows you the effect on the geometry and it will also update the Variable Table with the new value.

The following is just one example of how to use the Goal Seek command to aid in model creation. This example illustrates how to use the Goal Seek command to help design a sheet metal cover.

Note:  For this example, we have to create a hole pattern, on the top of the cover, to allow for air flow. From previous analysis it’s been determined that we need a minimum open area of 6000 mm². To achieve this we will start by creating a circular cutout and rectangular pattern.

I first create and position a 10 mm radius circle, as shown below, to create our initial cutout.

While still in the sketch environment, I select the Area command, from the Inspect tab > Evaluate group.

I then click in the area of the circle.

I accept the Area by selecting the green checkmark on the command bar.

Next I open the Variable table and locate the Area variable and rename it to Cutout_Area.

 

I also locate the 10 mm variable for the circle radius and rename it to Cutout_Rad.

I then close the Variable table and complete the cutout using the Through All extent option.

Next I create a Rectangular Pattern, as shown below, using the Fit option with the following values:

  • X: = 10
  • Y: = 5
  • Width: = 170 mm
  • Height: = 65 mm

 

The completed pattern should look like the image below.

To prepare to use Goal Seeking I need to create some User Variables. First, I find the X and Y occurrence variables and rename them to X_count and Y_count.

Next I create a Total_Area variable by clicking in an empty row and selecting the area type, from the pull down scroll, as shown below.

I then type in the name Total_Area and tab over to the Formula column. In the Formula column enter the following formula:

                      Cutout_Area*(X_count*Y_count)

 

Note:  I have now created a variable to calculate the total open area created by the pattern. I can now use this variable to help adjust the cutout radius to obtain the desired area of 6000 mm².

To do this I select Goal Seek from the Inspect tab > Evaluate group.

The Goal Seek command bar will appear.

I select the Goal Variable, which is the Total_Area.

I then select the variable that I will allow to change to obtain the Goal variable, which is the Cutout_Rad.

Now I enter in my target value of 6000 mm². (I just have to enter in 6000)

Note:  Goal Seek will now run through a series of iterations, where it will adjust the cutout radius, until it obtains the target value. When it is complete, it will show you the finished model, and post the number of iterations it used and the total elapsed time it took, in the bottom on the Status bar.

If I open the Variable table and view the User Variables, I can see that the radius of the cutout is changed from 10 mm to 12.36 mm, and our total area is now 6000 mm².

Using the Goal Seek command allowed me to determine the optimal radius for my holes without having to do any advanced calculations.

For more practice, try the Solid Edge tutorial on ‘Using Engineering Calculation Tools in Solid Edge.

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Using the mouse to manipulate the model view in Solid Edge

Thursday, June 21st, 2012

The middle mouse button, or scroll wheel, provides improved model rotation in ST4. You can now select a vertex, edge, or face as the model rotation center. To do this, simply following the steps below:

First you must let the system know that you want to enter the rotation mode. This is achieved by a single click to the middle mouse button (MMB), on an empty space. You will notice the cursor changes appearance. Before you click the MMB your cursor looks like this:

                    

After you click the MMB you cursor will look like this:

  

Notice that the little blue face, indicating selection mode, has disappeared.

You now have three options available to you: 

 

1. Rotate using a position on a face.

  •  - You can now move the cursor over the face shown below. Notice the dark pink dot, indicating that you are in the rotate mode.

 

  • - If you now hold the MMB down, the part will rotate about the dark pink dot. In other words, the dark pink dot becomes your center of rotation.

 

2. Rotate using a position on an edge.

  • - You can move the cursor over any edge. Notice the entire edge highlights.

 

  • - Holding the MMB down allows you to rotate about the edge. In other words, the edge becomes the axis of rotation.

 

3. Rotate using a position on a vertex.

  • - You can move the cursor over any circular edge. Notice the entire edge highlights.

 

  • - Holding the MMB down to rotate allows you to rotate about the vertex of the circular edge. In other words, the vertex of the circular edge becomes the axis of rotation.

 

Note:  Once you have completed the rotation, you are returned to selection mode. You will have to single click to the middle mouse button (MMB), on an empty space, if you wish to perform another controlled rotation.

 

Other handy mouse controls in Solid Edge

 - Pan the view. Press the Shift key while you drag the MMB to pan the view.

 

- Zoom. Scroll the mouse wheel to zoom in and out.

 

Note: The setting for this scroll behavior is found in Solid Edge options_Helpers page. Enable Value Changes Using the Mouse Wheel. If this option is on, the mouse wheel changes the value in a value edit field. Use Ctrl+mouse wheel to zoom in or out.

- Zoom Area. Press the Alt key while you drag the MMB to zoom into an area.

- Double–click the MMB: Fits the view.

 

Creating insert notches in sheet metal

Thursday, May 17th, 2012suggest

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.

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NX – Modeling a tapered thread

Friday, May 4th, 2012content

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.

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Simplifying the placement of certain dimensions in Draft

Tuesday, April 17th, 2012

Recently I had a customer contact our support line, looking for an easier way to place some dimensions. He was self taught on Solid Edge and was attempting to place the following dimensions on a formed tube.

 

 He had figured out how to do this by creating and using extra sketches, but felt there should be an easier way to achieve his desired results. I walked him through the process, and felt that this would be a good tech tip to share.

To place the 2 dimension shown, do the following:

1. On the Sketching tab, in the IntelliSketch group, make sure that the intersection option is toggled on.

 

2. From the Home tab, in the Dimension group, select the Distance Between command.

 

  •  
    • - Make sure your option is set to Horizontal/Vertical on the command bar.

 

  •  
    • - Move the cursor over the bottom centerline so it highlights. DO NOT CLICK

 

  •  
    • - Now move the cursor over the angled centerline and hit the ‘I key’ on your keyboard. (I is for intersection)

 

  •  
    •  - Then move the cursor over to the vertical centerline and click.

 

  •  
    • - place the dimension.

 

Note: Hitting the ‘I key’, tells the system to find and select the intersection point between the 2 highlighted lines. If more than one intersection point is possible, a list window will appear allowing you to select the desired intersection point.

3. From the Home tab, in the Dimension group, select the Angle Between command.

 

  •  
    • - Make sure your option is set to Horizontal/Vertical on the command bar.

 

  •  
    • - Select the horizontal centerline at a non-keypoint.

 

  •  
    •  - Select the vertical centerline at a non-keypoint.

 

  •  
    • - Place the dimension.

 

Note: the trick here is to not select the lines at keypoints (endpoints or midpoints).

There are several hot keys and various command options, which assist in placing dimensions in sketches and draft files. Take the time to review the help section on each dimension command and you will save yourself a lot of time and frustration.

How to add an attribute column to a BOM in NX

Tuesday, April 3rd, 2012suggest

In the part attribute, I’ve created the Plist attribute, make sure you have the object selection set to “apply to component as part attribute” if you want to save the information in the part, otherwise use the “apply to occurrence in the assembly”.

In the part list I’ve created a new column and did a RMB on the full highlight column

Select Style and go to the column tab.

Click on the arrow.

Select Plist from list and OK twice.

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