Common Support Calls in September '11
Welcome to the second edition of this, the Innova Systems Technical Support Newsletter. Our Technical Support team have been working hard, compiling some tips and tricks to handle some of our more common support queries. If you missed last month's, catch up here.
Technical Support Manager, Ed Hawkins answers this month's ten most common support calls...
- Sheet metal option - "trim side bends"
- Shaded drawing views appearing dark or black
- Moving a drawing view, or table, onto another drawing sheet
- Showing trailing zeros in a drawing
- Upgrading The SolidWorks Workgroup Vault
- Turn Sketch relations on or off
- Applying a custom mesh appearance
- How do you increase the quality of PDF output (In drawings)?
- Hide/Show edges in drawing views
- Custom properties
1. Sheet metal option - "trim side bends"
The "trim side bends" option within a sheet metal
feature is often overlooked. When you have two flanges meeting each
other, we often get a nasty looking overlap like this:
If you take a look at
the property manager for either edge flange, there is a tick box underneath
“flange position” called “trim side bends”. When enabled this will allow the
corner to be relieved, opening up the bend region and stopping any overlap of
the flanges occuring.
2. Shaded drawing views appearing dark or black
A recent problem has been reported in 2011 SP4.0 where shaded drawing views have been appearing very dark – almost black in appearance. The problem relates to realview graphics, and there are two solutions. One is to give us a call on Technical Support and we will send over a hotfix for you to apply. (N.B. This hotfix must be removed prior to upgrading to 2011 SP5.0 or 2012) The second option is to turn off RealView graphics.
3. Moving a drawing view, or table, onto another drawing sheet
Although this is actually a
very straight-forward process, it often causes confusion. So, you have multiple
drawing views on one sheet and you want to move one to another to make some
more room. Access the first sheet with the view you want to move on, right
click the view (keep the right mouse button held down) and drag this view
inbetween “Sheet2” and “SheetFormat2” in
the property manager. This will move the view onto the second sheet and keep it
in the same position as it was.
Now, dimensions show with the correct precision according to the document’s settings. You can manually override the precision on dimensions by selecting the dimension and changing the “precision/tolerance” field.
4. Showing trailing zeros in a drawing
More often than not, your drawings will be set
to show no trailing zeros. For example, if a dimension is a whole number, like 50mm, the
dimension will read “50mm”. However, a lot of people drive their tolerances
globally – with a note on the drawing referring to the no. of decimal places. In these cases, not showing any trailing zeros causes a problem. To turn on trailing zeros,
simply go to the tools menu, then to options, then click on “document
properties” and select “dimensions”. You will then need to switch the trailing
zeros option to “show” not “smart”.
This will now mean that dimensions show with the correct precision, in accordance with the document’s settings. You can manually override the precision on dimensions by selecting the dimension and changing the “precision/tolerance” field.
It is worth noting here that we have changed the options for the current document - not all documents. To retain this change for all future drawings we need to save this as a drawing template (.drwdot). To do this, click file, then save as, then change the file type box to “drawing template(.drwdot)” and overwrite the template you were using.
5. Upgrading The SolidWorks Workgroup Vault
With the release of SolidWorks 2012 just around the corner, I thought it would be worth talking about how easy it is to upgrade your PDM Workgroup server installation. We get a lot of calls on this, but if you follow the instructions below, you can upgrade it yourself (we are always on-hand to assist with this if you are still not sure).
Firstly, you will need to be logged on to the computer that is hosting the vault (you can find out what this is by using the vault window inside Solidworks - it will say the computer name followed by your login name at the top of the screen).
- Stop the Workgroup service – this restricts anyone from accessing the vault while the update occurs.
- Make a backup of the vaultdata folder - just in case!
- Insert the Solidworks DVD (or you can use the downloaded files) and browse to the folder called “pdmserver”. Within here will be an installer file called “Solidworks Workgroup PDM Server”.
- Double-click this file. This will launch the installer.
- Follow the instructions in the installer window, it will detect that you have a previous version of the software and suggest you upgrade.
- Once the install is completed, make sure the Workgroup service called “PDMWorks Workgroup Server” has started again on the server. This may launch a progress bar – wait for this to finish.
6. Turn Sketch relations on or off
We often advise new users to
ensure that sketch relations are turned on because it is very useful to see what
SolidWorks is creating for you automatically (like vertical and horizontal).
However, if you have a complicated sketch, they can be quite confusing and
annoying. If you want to turn them off you can go to the tools menu and de-select
sketch relations. Alternatively, you can take advantage of the heads up view
toolbar and select the relations icon
from the drop down.
7. Applying a custom mesh appearance
In the "Surface Finish" tab of an appearance there are two predefined mesh patterns - "circular hole mesh" and "diamond hole mesh". If neither these are suitable for the rendering it is possible to choose the "Custom hole mesh" surface finish type; this allows the user to use any image to create a hole mesh of any pattern.
Some tips for generating suitable images:
- Use a black and white image. Other image types are internally reprocessed as black/white.
- Black areas will be the "empty" areas of the mesh; white areas will remain rendered using the chosen appearance.
- For best results use an image format that does not reduce quality with file compression. JPG is not suitable, however PNG and BMP are.
- Create an image that can be tiled/repeated to create the mesh.
- Use a square rather than rectangular image for easier control of mapping (e.g 512 x 512 pixels rather than 640 x 480).
8. How do you increase the quality of PDF output (In drawings)?
There are a few ways to increase the quality of PDF output:
- Increasing the image quality slider to high in tools, system options, document properties, image quality.
- Enabling the high quality option in the save as PDF export options. This will go up to 600dpi.
- Enabling anti-alias edges/sketches in tools, system options, display/selection.
9. Hide/Show edges in drawing views
There have been some under-the-radar
changes with regard to hiding and showing edges in drawing views. These came in
a few releases ago, but are worth mentioning again. The easiest way to hide
or show edges is to click on a drawing view, and select the hide/show edges
tool, shown here:
This will give you a nice property manager on the left hand side with some automated options. Alternatively you can just select the edges you want to hide and click the green tick!
There are a few ways to add custom properties to a file – including the new custom property tab builder (available from the Windows Start Menu, under SolidWorks tools). But for those of you who still use the old fashion way – by going to file then properties, this is for you!
Do you always add you own custom properties by just typing them in or always hunt through the list to find the ones you want? If you do – then you can actually open the text file that populates this field and delete, or add entries to it. It is located here:
- Windows 7 – C:\Program Data\Solidworks\Solidworks 2011\lang\english
- Windows XP – C:\Documents and Settings\All Users\Application Data\Solidworks\Solidworks 2011\lang\english
All you need to do is open the file called “properties.txt” and modify the contents.