Archive for July, 2012

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Using Goal Seek to aid in model design

Thursday, July 19th, 2012

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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NX – Create a family of standard parts (Excel)

Wednesday, July 4th, 2012about

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

     1.  Create an 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 lenght 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.