Posts Tagged ‘Siemens PLM’

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Using Goal Seek to aid in model design

Thursday, July 19th, 2012careers

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.

NX – Create a family of standard parts (Excel)

Wednesday, July 4th, 2012
tools

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.

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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.

 

A new look pattern command in NX8

Monday, March 5th, 2012careers

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!

New to ST4 – a positioning relationship command: Range Offset

Tuesday, February 14th, 2012
tools

Now an offset can be created to control the range of allowable motion in relationships such as mate, planar align, axial align and more. This can be particularly useful when you wish to control or limit the motion of moving components. It allows you to prevent over extension, or collisions, of parts.

How to set a range offset

In the following example we want to set a range of allowable motion for the hydraulic cylinder, which controls the handle movement.

 

Step 1:       Apply assembly relationships as normal.

  • - Here we created an axial align and mate relationships, to position the moving part of the cylinder.

 

Step 2:       Edit the mate offset.

  • - Select the “Mate” relationship from PathFinder . Notice that it is a fixed relationship set at 20 mm.

 

  • - Click on the “Fixed” icon and change it to range as shown.

 

Note:  The “Range” toolbar appears showing first the current position (20mm) and then the range which starts at zero to 20.

  • - Set the range value. In this example, we changed the 20mm value to 50mm and select “Enter”.

 

Note:  You have to use the Enter key or it will not take the entry.

Step 3:       Test the range setting.

  • - Select the drag component command and use the “Freeform Move” option.

 

  • - Drag the black handle back and forth and notice that motion is limited by the range that you set.

 

  • - The handle now has a 50 mm range of motion.

Note:  Range offsets are not intended to be used for geometric tolerances, as over constrained components can occur.

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How to measure a volume enclosed by assembly parts or cavity in NX.

Thursday, February 2nd, 2012

In the following assembly I need to find the volume inside the gearbox, by using SPACE FINDER from the Analysis menu.

When specifying the interior point, make sure that the point is in the space that we need to measure and not on a face. Select the part making a close environment

 

 

The space finder also create 2 datum plane specifying the minimum and maximum, this information helps us define the maximum height of volume needed using the volume-height analysis section.

 In this section you can specify either you maximum height or volume and save it has a faceted body.

This is a fast and easy way to evaluate the quantity of liquid needed, for more precise evaluation other tools are necessary.

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