Questions and Answers
Q: Keyboard shortcuts: I'm trying to define keys for customization, but every time I go back in to add more, the older ones get wiped out. Why don't they stay put?

A: One possible cause may be that you have more than one instance of Solid Edge open. The settings are only written to the registry once Solid Edge closes properly. If you have more than one instance of Solid Edge open, the settings of the last instance will override the previous settings.

Q: Draft, Parts List: The parts in the BOM shows a 0 quantity for some parts. The "parts list count" callout on the part also shows a 0 quantity. The material and other information on the part is correct. I am using Solid Edge V20.2.

A: I am not sure whether or not this is a bug. In the specific case the parts list was done on an exploded view which was not saved under the view configuration. Once the view configuration was saved with a specific name (e.g. "MyExplode") this resolved the problem. (In the Explode-Render-Animate environment go to Tools > Configuration > View Configuration and enter a name and save it.)

Q: Assembly: I cannot move any parts in my assembly. The parts are not fully constrained, but the "move part" button is disabled.

A: It is likely that you have broken relationships in your assembly indicated by a red lighting bolt next to the relationship. Fix this and the move button will appear. Alternatively, if the move button is enabled, the parts that you want to move may be in a sub assembly. Open the sub assembly and move the parts in there.

Q: Frame Design: I want to make changes to the individual members of the a frame (e.g. cutouts, etc). How can I do this?

A: Right click on the frame component (e.g. "Frame1") and select the "save as" option. This will export the frame as an separate assembly with parts, which can be edited. If you open the assembly it may appear empty (i.e. no material with BOM present). Open the individual parts and right click on the part copy feature. Select the "make base feature" option to change the part copy into material.

Q: Frame Design: I have created my own part that I want to use as a cross section in a frame design. One of two things happen: I get a message "The standard parts library contains no frame components" or the cross section of the frame has the wrong shape.

A: A part file that is used as a cross section in a frame must contain only one protrusion (and nothing but this one protrusion, sketches excluded). The error message appears if there is no protrusion in the part.

Q: Standard Parts: I have installed the Standard Parts administrator but, I do not see all the parts that should be in the Machinery (or piping) Library.

1. Install the Machinery Library (or piping library) from DVD or CD. (It will appear on Add & Remove programs list in the Windows control panel once it has been installed).
2. Run the Configuration Wizard. (You can use the default settings.) Start > All Programs > Solid Edge V20 > Standard parts > Configuration Wizard.
3. Run the Administrator and register the new parts in the database. Start > All Programs >  Solid Edge V20 > Standard Parts > Administrator. Click on the "registers parts" (or "add parts") button. Follow the wizard to register the parts in the machinery/piping library. The registration process should typically take 4 hours to complete.

Q: In the assembly environment I am not able to change a part's material (using Tools > Property manager). I opened the part itself and also cannot change the material type.

A: Check the following:
1. Make sure the part is not read only.
2. Make sure the part is not a "part copy" of some other part. If it is, you can break the link between this part and the original by selecting the "Part Copy" feature in the part, editing its definition by going to its options dialogue and un-checking the "link to file" option.

Q: My template draft files are very large (> 1MB). Why is this and what can I do about it.

A: Check the following:
1. Make sure that the images (if applicable) that you are using for your company logos are small. GIF files are ideal for logos as GIF files are space efficient for small images with less than 256 colours. Resize the images to the correct number of pixels before inserting it into Solid Edge.
2. Some users use relationships on their background sheets' borders (e.g. connect, horizontal/vertical alignment, locked, etc.). These relationships makes the files very large. Remove the relationships unless your really need them.

Q: When I save my Solid Edge draft / drawing files to AutoCAD dwg format, the text looks different. What causes this and what can I do about it?

A: Solid Edge uses a set of fonts (which are installed as standard Windows fonts) but some AutoCAD versions do not recognize these fonts. Do one the following:
1. When saving the file, on the "Save As" dialogue box, select the options button. You can change the font translations so that the Solid Edge fonts are translated as say Arial Narrow.
2. You can change your Solid Edge file (especially your template) to only use well known fonts like Arial.

Q: I want to change the Dimension Style from Fractional ANSI(Inch) to decimal ANSI(Inch) in Solid Edge V19.

A: Click here to read the detailed answer.

Q: The Problem I have is that I'm receiving drawings from Europe and I need to change all the dimensions from metric to US standards in Solid Edge V19. Is there any way I can change all of the dimensions at once instead of picking each one and right clicking and changing it under properties?

A: Click here to read the detailed answer.

Q: When I stitch surfaces Solid Edge doesn't give make a solid body (or material).

A: Check the following:
1. Make sure that the surface forms a closed (and non-intersecting) surface body
2. When using the stitch command make sure the all the relevant surfaces are selected and that you use the heal option. Increase the tolerance on the heal if necessary. (The heal option fills small holes in surfaces which may result from numeric representation of curves and surfaces.)
3. Ensure that there is no material (e.g. protrusions) in the model. Solid Edge will not allow you to create a base feature through the stitch command if there is already material in the model. It is not sufficient to simply suppress any material commands, they should be deleted.

Q: In the main screen, if I click on drawing, it enters the 2D environment and works properly. But, if I click on either solid part or assembly, I can see only the toolbars, but not the working screen. What may be the problem and what's the solution for this?

A: Click here to read the detailed answer.

Q: How do I get a parting split on a molded product where the parting doesn't take place in a flat plane.

A: Click here to read the detailed answer.

Q: We have discovered a mistake in the bending direction of the bends are reversed ("up" and "down" is swapped around). This occurs when placing views of flattened sheet metal parts in Solid Edge (Version 20) and adding a bend table.

A: Click here to read the detailed answer.
A: Please note that there was a bug in Solid Edge V20.0 to V20.2. Load SP3 or later for V20 to fix this.

Q: When I created a cutout with draft treatment on it, the draft treatment happens in the wrong planes or sides.

A: Please note that when you use the treatment step on a cutout (or protrusion) the draft happens in the same direction as the cutout (or protrusion). If you want draft treatments in a different orientation, use the draft command.

Q: When I created flanges in the sheet metal part environment, Solid Edge does not create bend relieves.

A: 1. A bend relief will not be created if the relevant flange will not result in material tearing. Therefore make sure the bend of the flange falls with the material (and not outside it).
2. When creating a flange, select the flange options button on the Solid Edge ribbon bar. Ensure that the "Bend relief" checkbox is selected.

Q: I have text on the buttons, but it appears larger than it ought.

A: The size of the text can be changed when using some NVidia Quadro FX cards. (Right click on the desktop wall paper, select properties, select settings, click on advance, click on the Quadro FX tab and go the appropriate setting.) To take the text off the buttons then start Solid Edge - open a new document, go to Tools > Options > Helpers > "Text on buttons"

Q: My model appears to have a strange perspective on it (in the asm/part environment)?

A: You can change the perspective on the model with ctrl+shift+roll the mouse wheel.

Q: My 3D sheet metal model doesn't want to flatten.

A: 1. Ensure that there are no flanges intersecting one another so that the part can flatten.
2. Ensure that there are no ruled surfaces in the model. The sheet metal part you designed may contain a ruled surface. All surfaces in a Solid Edge sheet part must be developable. That is, it is "surface" which can be flattened onto a plane without distortion (i.e. "stretching" or "compressing"). Think of a car bonnet for example. In order to make the bonnet of the car the blank, flat material must be “smeared” resulting in a non-uniform material thickness. Solid Edge cannot develop parts like that as it requires extremely complex calculations.
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