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Showing posts with label assemblies. Show all posts
Showing posts with label assemblies. Show all posts

Monday, 29 February 2016


Often times, in SOLIDWORKS, we will need to apply multiple mates of a similar type in an assembly. There is an option called SOLIDWORKS Multiple Mate Mode that can accomplish this. This process works with all kinds of mates, but it’s easily demonstrated here with the concentric mate. Please consider the following assembly:
I'd like to make everything concentric to the bolt
I’d like to make everything concentric to the bolt
Looking at the assembly, there is one bolt, 3 washers, 3 lock washers and 3 nuts. Using traditional mate selection methods, you would require 18 selection clicks. What if I told you it could be done in 10? Let’s check it out. If I launch the mate command from the toolbars, I take notice of the button indicated:
Multiple Mate Mode
Multiple Mate Mode
Using this button changes the interface on the side a bit. It allows me to select one as a common reference (in my example, the cylindrical face on the bolt) and then select as many other references as I like (a cylindrical face on each of the other components). Behold:
SOLIDWORKS Multiple Mate Mode
Applying a Multi Mate
This is likely enough for most people, but it you want to get really fancy, there’s a checkbox for “Create multi-mate folder” that you might notice in the above screenshot. Here is what that option does:
Multi-mate folder
Multi-mate folder

Thursday, 15 October 2015


When a SOLIDWORKS assembly file will not save the first workaround is to try and save the assembly with a new name, to a different folder, or to a local drive.  If that doesn’t work then here are two other options for you to consider trying.
Note that pattern and mirror features cannot be included in these steps in the versions prior to SOLIDWORKS 2016; they would need to be recreated.

Option #1: Form a New Subassembly

Selecting assembly components, right-click and select the option ‘Form New Subassembly.’  Once the new subassembly is created, try saving it externally.
SOLIDWORKS Assembly File will NOT Save
Form New Subassembly and Save Assembly in External File (RMB = Right-mouse Button)

Option #2: Make Assembly from Part/Assembly and Dissolve Subassembly

From the File menu, select Make Assembly from Part/Assembly.  SOLIDWORKS creates a new assembly with the original assembly as a component.  In the new assembly, right-click on the subassembly component and select the option ‘Dissolve Subassembly.’  The result should be a replica of the original assembly that may not report an error when saving.

Make New Assembly and Dissolve
Make New Assembly and Dissolve

Wednesday, 7 October 2015


Perhaps you work for a company that makes use of SOLIDWORKS custom properties. Of course you use them, they’re terrific for populating your BOM automatically and can be used for a whole host of other purposes. However, the custom properties that you use at your company are very special — one might almost say…custom.

Let’s say your company always uses four custom properties on your BOM: “Description,” “PartNo,” “Supplier,” and “Material.” However, when you download an air cylinder off of a supplier’s webpage, they do not have the same custom properties. You could populate these manually, but that would be time consuming — especially since you know that they will need all 4 properties, without typos. Did you know you can copy and paste a list of custom properties?
Copy and Paste SOLIDWORKS Custom Properties
Custom Properties dialog: select the row “1” then hold shift and select row “4”

The Copy & Paste Process

  1. First access the custom properties from File > Properties
  2. Then, select the list of custom properties from a source file by selecting the row header (where it says “1” on the left), then hold down the Shift key and select the last row (“4” in the example above). You can also use Ctrl+select to select specific properties, just as you would in Windows Explorer or the SOLIDWORKS feature tree, or many other programs.
  3. Then give it the old Ctrl+C to copy it.
  4. You can then exit the dialog window
  5. Open the new file and access the custom properties dialog and
  6. Paste the properties (Ctrl+V) into the dialog. Tada! All your custom properties now appear in the new file.
True, they are populated with the same values, some of which may need to be manually changed, but this is far, far, faster than having to recreate the properties manually.

Wednesday, 16 September 2015


Have you ever jumped right into building a model, selected a plane to begin sketching your best profile onto and then, some way into modelling felt that your models view orientations are just not quite set-up right? Perhaps you have found yourself in the drawing environment whilst pulling model views into a drawing and have noticed that certain view orientations don’t match up by name to how you thought they might?

Well here is an incredibly simple reminder of how to re-orientate your standard views in SOLIDWORKS for the many reasons that you may want to do this.

In the View Orientation drop down menu we have a variety of options for orienting your model in three dimensional space. We have 6 standard projection views and 3 standard perspective views. We can also orientate the graphics area Normal To/Perpendicular to a selection that you have made as well as the ability to tile multiple model view orientations across the display area. We can also add new custom views and use the view selector. I would like to view the front of my model now and so have went ahead and selected the Front view in the view orientation drop down. SOLDIWORKS will now rotate and zoom my model to the selected view orientation.

This orientation however is not reflective of what I would consider to be the Front of my model. I would consider the screen of my tablet model here to be the true front of it and as such would expect the Front View to match this preference.

For this reason I would like to reset the standard model views to reflect my preference and can do this by clicking the view orientation box in the heads-up view toolbar and selecting the more options arrow to the top right of the menu. I can also access this menu via the (Spacebar) keyboard shortcut or by navigating to View > Modify > Orientation.

Once inside this menu I can make changes to my view orientations by either clicking on Update standard views or Reset standard views. Resetting will allow me to revert to the original views if I make any changes that I would like to undo. Update standard views will let me make changes to my standard view orientations. I will click on Update standard views in this case.

SOLIDWORKS will then ask me to select the view that I would like to assign the current view to. But what is the “current view” that SOLIDWORKS is referring to? Simply, whatever orientation I currently have my model placed in on my screen. That orientation will be assigned to the standard view that I select in the menu. So be aware that you could orientate your model in any way, Normal To a particular area of the model or indeed completely arbitrarily if you wanted to.

I have now orientated my model to what I consider to be the bottom of the Tablet and as this is my “current view”, upon selection of the standard bottom view icon in the view orientation menu, my “current view” will be assigned to this. SOLIDWORKS will now inform me that various other views will be affected if I assign this new view orientation to my model. Happy that I am ok with this, I will select yes to proceed.

Whenever I do this, all of the standard views will be updated based upon the re-assigned bottom view. The comparison given below shows the change that this will now make to each of the standard views. I managed to divide my screen like this by selecting the Four view tile option in the view orientation menu.

The image above displays my original model orientation and the image below, the new. Pay particular attention to the name of each view orientation. ie. *Front, *Left, * Top, *Isometric.

I hope that you can find a use for this month’s very simple tech blog or that it has solved any headaches that you may have had when orientating your model in the display area. The benefit of making these changes helps you more intuitively flow between model views and extends into the drawing environment as well which can save any confusion between drawing view names and their orientation.

Tuesday, 15 September 2015


In a previous blog, “How to create a library design feature in SOLIDWORKS”, we saw how we could create library features, now we will look at how we can take those library features and incorporate the new and improved patterning tool options that were introduced within the 2015 release of SOLIDWORKS. As many users have already found the new options very useful we have tried to push the limits of the new options and have found some very useful ways in which they can be used. In this blog we will look at how we create these intelligent library features by using the new patterning tools and how we can apply these to our parts. In this blog we will use a set of simple cut outs and bodies to demonstrate intelligent library features.

CREATING THE LIBRARY FEATURE:

We do not need to do anything special to create these library features, they can be created in the same way as normal library features but just incorporating the patterning tools. The first step is to create the design required, in this case some simple cuts and bodies.

Firstly, just like smart components, we need a defining part file. This will be where we define the library feature and choose what features or bodies we will use for a library feature.
So in this scenario we will create a worktop with simple cut outs and bodies to fit into the cut outs. We have created a base worktop with a secondary worktop that sits above it with a cut out through both worktops and a container that fits into the cut out.
Library_1

Library_2

We now need to apply the patterning feature with the spacing options needed. As we have placed the container in the centre of the worktop we will be using the pattern seed feature option. We will first pattern the cut out and then the container.

 Within the patterning tool if we select our direction 1 and 2 as the same edge and choose out pattern seed feature, we specify our spacing options for each direction.
Library_3
Next we will choose the new options for Up to reference in each direction. This will allow us to use a offset edge to control how far in the pattern will be from the edge specified and this will also build intelligence into the part, as we increase the length of the worktop the pattern will increase or decrease, giving us more or less cut outs in the worktop.
Prior to SOLIDWORKS 2015 and this enchantment in particular, users would have to create a pattern and then use a function within the modify dialog box to make the intelligent update work, Increasing the workflow steps required and also the time involved in creating an intelligent model.
Library_4

Once the user has set clicked ok the intelligent pattern has been created. To test this, the user can change the overall size and see the parts start to update. In this example we have set the dimension reference or the upper worktop from the edge of the lower worktop so as we change the size of the lower worktop the upper will change automatically.
Library_5

We have repeated the previous pattern for the container but just pick the bodies to pattern instead of features to pattern to achieve the desired result.
Library_6
If we increase the size of the lower worktop from 400mm to 600mm we will see the pattern increase the cut out and containers to 5 instead of 3.
Library_7
Using these great tools has allowed us to quickly create the desired effect. Now we will go on to create the intelligent library feature.

 Just like creating any library feature, if we select the features we would like in the library feature from the feature tree we can then save the desired features as our library features from the normal save menu but picking the Lib Feat Part (.sldlfp) from the Save As Type list.
Library_8

Library_9
This will then save all the features required as a library feature file we can then use in any part. We would ideally like to put these library parts into a common folder that we can access. Once in this common folder we can set a folder location in the design library to always see these newly created library parts.

USING THE INTELLIGENT LIBRARY PARTS:

 We have set a folder location on our design library to show all the intelligent library features we have created, including the one in this blog. We have done this by using the Add File Location button on the design library in the task pane. We will now use the created library feature within a new part.
As an example we have created just a rectangular boss 800mm X 200mm in a new part file.
Library_10

We will now drag and drop our newly created library feature from our design library location
Library_11
Once out Placement Plane has been selected, we can now start setting the references required. This will be the edges used to create the upper worktop. The preview window will show what edges, faces or sketch points to pick.
Library_12
As we can see the library feature has updated and added an extra 2 containers and cut outs to the desired worktop.

 If we take the 800mm length down to 400mm the extra 4 containers reduces, this build our intelligent library feature.
Library_13
A fantastic way to automate feature and body creation as well as allowing the user a quick and easy way to develop the design as requested. Using intelligent library feature within a design could save a lot of time, effort and development of a product. This is one of the many way the new options within SOLIDWORKS 2015 can help users create some very dynamic parts.

Tuesday, 1 September 2015


Hold down your right mouse button and slowly move your mouse pointer. The ‘wheel’ that appears on your screen is the in-context mouse gesture shortcut toolbar, and each of the icons is a shortcut.
Just swipe the mouse pointer over an icon and you will instantly access that command. The gesture wheel is fully customisable, so you can have up to 8 different shortcuts, and its in-context, so you see different shortcuts if you are in sketch, part, drawings or assembly mode.
Techie_1

Techie_2
 To customise the wheel, right click on the command manager toolbar and select Customize:
Techie_3   Techie_4
 Select the Mouse Gestures tab, here you can select 4 or 8 wheel gestures.
Techie_5
Tip: A slow double click on the column title will sort already set shortcuts.
Techie_6To set a shortcut either scroll down the list or use search tool to find the command you want, then click in the relevant column and cell to set its wheel position:

Techie_7
After a bit of practice and as you start to remember the wheel positions you will become faster and more productive, you can also print the gestures list out and keep a copy by your machine (ensure that “Show only commands with mouse gestures assigned” is checked before printing):
Techie_8


 

Thursday, 27 August 2015


Sometimes it is useful to be able to create sketch geometry where items intersect, for example 2 bodies, or where a body and plane intersect.

In the image below we can see a sweep through which the front plane is located.


We can use intersection curves to show where in this case the body and the plane meet.
To do this, firstly start a sketch on the front plane, and then select either the intersection curve icon from the drop down arrow under the convert entities button on the sketch toolbar, or select it from the ‘Tools/sketch tools menu’
 


Now select the geometry you wish to generate the intersection for.  I have selected the body from the ‘Solid Bodies’ folder in the tree but you can select features, faces and so on as required.
 Result:


You can also do this with intersecting bodies, and you don’t need to be in an active sketch, for instance in the below example we will generate the intersection between the red and grey bodies.


Simply start the intersection curve command and then select all the faces that you wish to see the intersection of.

Result. A 3d sketch is generated with the intersection sketch geometry.

 

Wednesday, 12 August 2015



A SOLIDWORKS Global Variable is a useful way to keep a set of values linked to dimensions in your model so you can quickly make a change and all dimensions linked will be updated.  But perhaps you are adding a dimension and you just want to enter the value of one of the Global Variables without linking it.  This way the dimension will not be affected by changes to the Global Variable.

Rather than linking with an equals sign, “=”, to the Global Variable…
Linking to SOLIDWORKS Global Variables
Linking to the Global Variable with an “=” sign
Instead you can just add a plus sign, “+”, and it will give you the drop-down to select the Global Variable.
Adding Global Variable Values
Only Adding the Global Variable value with the “+” sign, without Linking

The value of the Global Variable will be added, but the link will not be put in place so it won’t be affected by future changes.

Here is a video demonstrating the differences:

Monday, 6 July 2015



It can be quite a time consuming process creating renders, the process of tweaking settings in search of perfection can easily swallow time. The following tips are not only intended to help improve the quality of your renders, but also reduce the time taken to get to the final stage.
1
1. Rotating the environment

 Quite often it is advantageous to put lights into your render, they will help to illuminate your model in desired areas and will create attractive highlights across your design. However, more lights means more reflections, more reflections means your render will take longer to output. When setting up a render it can sometimes be a good idea to avoid lights if under pressure to complete work. This makes it challenging to get an attractive output.

As an alternative to this technique; rotating the scene to differing angles in order to improve the look of a design can work wonders. It will help to improve the look of a model, by moving the position where highlights strike the edges of a product. This technique will not increase render time either, keeping things nice and simple. This can be adjusted by going to the Display Manager, navigating to Scenes, Lights and Cameras and editing the Scene.

2. Applying appearances which “look Right”

Under the Task Pane there are a wide variety of appearances available. Quite often you can find the exact appearance for the look you’re going for. However, these can sometimes not quite look right once applied. There are a variety of reasons for this, but quite often it can be attributed to the scene being used. Different scenes can make appearances look entirely different.

2A better way of working is often to apply the appearance which looks correct. Rather than the exact appearance specification created for a material. For example; I have found that the high gloss plastic can work well for any glossy painted surface, it doesn’t necessarily have to be plastic.

3. Appearance alternatives

Sometimes the desired appearance isn’t available. In some situations this means making do with an appearance which doesn’t suit the rendered design at all. Rather than trying to tweak an inappropriate material to make it fit the look of your design it can often be a much better idea to download an alternative. There are two possible options here;
3
You can look online for free texture maps online- You will often find that a pleasing result can be achieved by searching for free texture maps for the appearance you want. This technique allows you to achieve pretty much any appearance. Once the appropriate image has been found online it can be applied onto your model by dragging on the default Texture appearance, which you can find by clicking on the appearances library in the task pane. You can edit the appearance and change the image to any image that can be downloaded.
If you are a subscription paying customer you can access appearances online through the customer portal. There is a link to Photoview 360 Appearances, by following this you can access luxology’s online library of appearances. These can be downloaded and used within SOLIDWORKS. There are some really good appearances in here, it is worth checking out.

4. Creating Depth of Field

Depth of field is one of those things that will differentiate your render, and make it appear as if it has been shot on a high quality SLR camera. In order to use these settings in SOLIDWORKS you will first have to create a camera view.
4Camera views are a brilliant way to save a view and easily edit the perspective shown on your design. They are accessed under the Scenes Lights and Cameras in the Display manager. If you have Photoview 360 turned on when creating your camera you will be able to edit the Depth of Field options. Once ticked on the best way to set this is using the Focus by selection option. This option allows you to select your model in the area you want to focus. Once set the important option is next to the f symbol, This is your F-Stop. In a camera this would be like altering the aperture, so small numbers give the smallest depth of field.

5. Creating a reusable render setup

 One way to create a setup which can be reused over and over again is to create a standard render assembly, with this technique models can be dropped in when a render is required. After a bit of experimentation with Photoview 360 you’ll discover which environments and setups work well, you may want to add your own background into the scene (This can be done by editing the scene, as described in section 1). You could also consider adding a floor appearance, this can be done by Right Clicking on the scene in the display manager.
5Once the assembly is setup and ready for a render, the assembly can be saved, just by going to file>save as. A model could be dropped into this setup as and when desired. A full set of mates may not even need to be added, you may find it easier to add one so the model is the right way round. By Right clicking on the model you can use Move with Triad, this will allow you to get the model to the best position visually. Once complete right clicking again will allow you to fix the model in position. You can then render your design.

Obviously there are a whole load of other options out there in Photoview 360. However, these tricks when used well in combination, are an excellent way to produce attractive renders while saving you precious time!