Posts Tagged ‘Solid Edge with Synchronous Technology’

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Quicksheets

Tuesday, November 20th, 2012

A “Quicksheet” is a template of drawing views that are not linked to a model. You can then drag a model from the Library tab or from Windows Explorer onto the template, and the views populate with the model.  If you have standard views on a particular size of drawing, for example, you can have the Draft preconfigured to populate itself based on the model you place on the sheet.

You will to need to set up a Draft sheet (but do not use production drawing as the drafting information will be removed upon save) with your views and other items such as Parts Lists.

1. Go to the SE Application button

2. From the Application menu, choose the “Create Quicksheet Template” command.

3. Save the file to a location and give it a name that easily identifies it.  It is best to place this on a network area other users can get to if it is useful to share the Quicksheet.   It is also best to locate it in a similar area to where the company templates for SE reside.

* Almost all view properties, including general properties, text and color properties, and annotation properties, are maintained. However, some display properties, such as selected parts display, Show Fill Style, and Hidden Edge Style, are not maintained.

Now a Quicksheet template has been created, but how do we use it?

1. Open your Quicksheet template (either through Windows Explorer or if you set up your User Templates and placed the Quicksheets in that location hit New>Quicksheet> and select your Quicksheet).

2. Drag and drop your desired Part or Assy onto the sheet from Windows Explorer or through the Library tab in Solid Edge.

3. Solid Edge will place the geometry and will be ready for the next steps.

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Accelerate tool design with a few simple surfacing commands

Friday, September 14th, 2012

After completing a 3D model of your design, it may be necessary to design some custom tooling for manufacturing. Solid Edge provides some very simple surfacing commands to aid in the rapid generation of tool design. For example, you may have to design a custom dimple punch or a dimple punch and die set. Let’s assume that you have to design a tool to create the dimple shown here.

For this example, I will just illustrate how you can quickly design the face of the dimple tool. In a new part template, I use the Part-Copy command to insert the sheet metal part containing the dimple.

I will insert this as a construction body.

Notice that I have several other options available to me, if needed, in the Part Copy Parameters dialog.

From the inserted construction body, I can copy the inside faces of the dimple. I select the Copy Faces command from the Surfacing tab > Surfaces group.

I select all the inner faces of the dimple.

I then hide the construction body and I am left with the inside surface.

Next I create a symmetric protrusion which encompasses the surface.

I then select the Boolean command.

With the default subtract option selected; I select the surface as my tool.

I then select the direction that I wish to subtract, or remove the material, from the protrusion.

The protrusion is trimmed from the surface, as shown.

I now have a perfectly matched solid to the inner dimple face. I can now model the rest of the tool.

Using the same procedure I could create a matching die if necessary.

Many users are unaware of the powerful surfacing commands in Solid Edge. As shown above, these simple yet powerful commands can significantly accelerate your design process. If you would like to learn more about surfacing, we offer training in our advanced modeling class (http://www.designfusion.ca//advancedmodelingcourse.php) or you could try the self-paced training course online at http://www.solidedge.com/spt/en/ST5/spse01560/book.html.

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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.

 

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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.

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Non-graphic parts in Solid Edge assemblies

Friday, March 9th, 2012

Assemblies often contain components for which there is no model required, such as paint, grease, oil, labels, and so forth. These non-graphic parts still need to be documented in the parts list and bill of materials that are created for the assembly. In Solid Edge, you can use the File Properties command on the Application menu in the Part and Sheet Metal environments to add custom properties to an empty part document. These custom properties allow you to define the required information for these types of parts. You can create two types of non-graphic parts: parts that require a unit type and quantity, and parts without a unit type and quantity.

 Types of non-graphic parts

Parts with a unit type and quantity

Some non-graphic parts require a unit type and quantity. For example, you may require four liters of oil in an engine assembly. You can create a part document named OIL.PAR, and then set the unit type, Liters, in the part document. Later, when you place the oil.par document in the assembly, you can set the unit quantity using the Occurrence Properties command on the Edit menu.

Parts without a unit type or quantity

Other non-graphic parts require no unit type or quantity. For example, you may require a small quantity of grease between certain parts in the assembly. These types of part quantities are usually documented “As Required” on a parts list or bill of materials. For these types of parts, you define the custom properties and the text string you want in the part document. You do not have to edit the occurrence properties in the assembly.

 Placing Non-Graphic Parts

Since non-graphic parts do not need to be positioned with assembly relationships, you can place the part in the assembly by holding the SHIFT key, and drag the part into the assembly.

 

Create a non-graphic part that uses units and value

This procedure shows you how to define custom properties for a non-graphic part that requires units, and a value for those units. Although no 3D model is required for these parts, they still need to be documented in a bill of materials or parts list. For example, you may require 4 liters of oil in an assembly.

Step 1. In the part document, choose Application menu→Properties→File Properties to open the Properties dialog box.
Step 2. On the Custom tab, in the Name box, type: SE_ASSEMBLY_QUANTITY_OVERRIDE.
Step 3. In the Type box, select Number from the list.
Step 4. In the Value box, type 0 (zero). Then click the Add button.                                                                                                                                 
Step 5. In the Name box, type: SE_ASSEMBLY_QUANTITY_STRING.
Step 6. In the Type box, select Text from the list.
Step 7. In the Value box, type the unit and number of decimal places you want. For example, Liters;4. Then click the Add button.           

Note:  You must separate the unit type and decimal places with a semi-colon (;). If the number of decimal places you want is 2, you do not need to enter a value for the decimal places.

To use the custom properties in an assembly, do the following:

Step 1. Place the part in the assembly.
Step 2. Select the part in the PathFinder tab or the graphics window, then on the shortcut menu, choose Occurrence Properties.
Step 3. On the Occurrence Properties dialog box, type the quantity value in the Quantity cell for the occurrence. Notice that the unit value you specified in the part document is displayed in the User-Defined Quantity column.

Tip:

  • - You can place a non-graphic part in an assembly without applying relationships by holding the SHIFT key, then dragging the part into the assembly.
  • - You can also set the quantity value using the Occurrence Properties button on the Place Part command bar.
  • - If you use many non-graphic parts at your company, you can create a template that has the non-graphic part custom properties defined.

 

Create a non-graphic part that is unit less

This procedure shows you how to define custom properties for a non-graphic part that does not require units. Although no 3D model is required for these parts, they still need to be documented in a bill of material or parts list. For example, you may require a small quantity of grease that on the parts list is documented “As Required”.

Step 1. In the part document, choose Application menu→Properties→File Properties to open the Properties dialog box.
Step 2. On the Custom tab, in the Name box, type: SE_ASSEMBLY_QUANTITY_OVERRIDE.
Step 3. In the Type box, select Number from the list.
Step 4. In the Value box, type 1 (one). Then click the Add button.                 
Step 5. In the Name box, type: SE_ASSEMBLY_QUANTITY_STRING.
Step 6. In the Type box, select Text from the list.
Step 7. In the Value box, type the constant text you want. For example: As Required. Then click the Add button.                                                       

 

To use the custom properties in an assembly, do the following:

  • - Place the part into the assembly. The “As Required” property is automatically recognized in the Occurrence Properties dialog box. To review the part’s properties, select the part in the PathFinder tab or the graphics window, then on the shortcut menu, choose Occurrence Properties.

Tip:

  • - You can place a non-graphic part in an assembly without applying relationships by holding the Shift key, then dragging the part into the assembly.
  • - If you use many non-graphic parts at your company, you can create a template that has the non-graphic part custom properties defined.

 

Set part properties in an assembly

  1.  Click a part or subassembly in the assembly.
  2.  Right-click, then choose Occurrence Properties on the shortcut menu.
  3.  In the Occurrence Properties dialog box, set the options you want to use.

 Tip:

  • - You can also set the part properties with the Occurrence Properties command on the shortcut menu when a part or subassembly is selected.
  • - When you select the top level assembly entry in PathFinder, then click the Occurrence Properties command, the entire assembly structure is displayed in a bill of materials format. You can use the (+) and (-) symbols to expand and collapse the assembly structure.
  • - When you select one or more parts or subassemblies, the selected occurrences are displayed in a table format that cannot be expanded or collapsed.
  • - If you need to change the properties of a subassembly, you must first check out all subassemblies where the occurrence properties are being modified. Then the documents can be saved and checked back in to Teamcenter.

*Text passages taken from Solid Edge Help files.

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New to ST4 – a positioning relationship command: Range Offset

Tuesday, February 14th, 2012

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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