SOLIDWORKS Tips & Tricks

Every year all resellers have a customer launch event where we showcase the new version of SOLIDWORKS. At Innova Systems we always try and add a little more value to the day by doing some breakout sessions on a number of different subjects. This year I was tasked with doing a “Tips & Tricks” session, which is normally very well attended. This often causes us a few issues, as things that we use on a daily basis, we don’t necessarily class as a tip or a trick. We have also done a number of this type of sessions over the years, and it’s always nice if you can try not to cover any old ground.

What follows is the written break down of all the tips I went through on the day, some of them you may know, some of them you may not. But hopefully you will find them useful.

If you find it easier, I recorded the session with examples, which you can find here. While there you can take a look at some of the other useful videos from the day – or our videos on why 2015 is such a great release! If you want to go directly to our 2015 videos click here.

Model Navigation

We’ll start out with some simple tips to help you navigate around your model. There is a triad (showing X Y and Z) in the bottom left hand corner of SOLIDWORKS. If you click this axis’ with a combination of the following key strokes, you can navigate your model in a number of different ways

Select X axis – normal to the screen

Select Z axis to return

If we select the axis pointing towards us, it gives us the reverse normal to

Select X (with SHIFT) rotates around the axis 90

Select X (with SHIFT + CTRL) rotates around the axis in reverse

Select X (with ALT) rotates by the arrow increments

Select X (with ALT then CTRL) rotates in reverse at the arrow increments

If we double click the middle mouse button (MMB) on a face we can rotate about that face

CTRL + 1 will give us a front view, and you can follow those shortcuts in sequence to get all the standard views

If we hold down ALT + MMB we can roll/ rotate normal to the screen

CTRL + MMB will allow us to pan

SHIFT + MMB will allow us to zoom

We can access any saved views by hitting the space bar – and we can save these to SOLIDWORKS so they are available in any model we open

Pressing F will zoom to fit

Sketch

We all know that you can draw a line using the click – click – double click method, but if you just want a single line, try pressing the left mouse button and dragging and then release. No need to double click

We can access previews views – using the previous view button on the heads up toolbar.

If you select a sketch tool, you can change the type by clicking A (so if you pick a center rectangle, you can change the style by clicking A)

We can turn a selection into construction lines by clicking the box on the right, but we can also use the shortcut ALT + C to change entities that are selected.

Suffix dimensions with unit system to convert on the fly (so if your template is in “mm”, type “in” after your dimension and it will convert it from inches to millimetres.

But let’s say I want to continue in mm, I can use the unit switcher to change my unit system from the bottom right hand corner of SOLIDWORKS

Double clicking on a non-active sketch will take me back into edit sketch mode.

You can use simple maths functions in here too 10/2 = 5mm

Double click the screen to exit the sketch

Selecting a sketch and dragging the arrow, will either add geometry or remove it, depending on where I select. At the top, will add, at the bottom will remove

If you drag the end point of a broken circle or arc, you can create a circle again from the arc we dragged

Holding ctrl and dragging then releasing ctrl will move an entity, and holding ctrl and dragging (keeping hold of ctrl) will perform a copy command

A left to right box select will select everything in the box, but a right to left select will select anything the box crosses.

When adding sketch relations, we may want an additional relation based on the entities selected, but the flyout box disappears when you select your first relation. If you press ctrl, it will bring it back allowing you to add additional ones

In the dimension box, you can use the MMB to increase the value by the arrow key increments. If you hold down ALT it will divide this increment by 10, or hold down CTRL to multiply by 10

Power trim is a great time saver – here we just need to drag our cursor through what we want to trim, and it trims back to the nearest boundary

If you accidentally trim entities you don’t want, you can restore them by going back through the black (or red, depending on your settings) box

We can also extend entities while being in the trim command, just drag an endpoint and it will extend

Features

When in a feature property manager, like “Extrude” a right click will give us access to the end conditions

Right click now is enter (as long as you don’t move your mouse!)

When you create a feature and accept the property manager, it is selected in the feature tree, clicking S will bring up the shortcut key, but it also starts the command search in the top right, I can just fill in circ and it will show commands with that text string it – circular pattern is what I’m after.

The feature automatically adds itself, and I can select any additional features in the normal way. Pre-selection is a great way to speed up the modelling process.

Useful Keyboard Shortcuts

Pressing HOME will show the top of the feature tree

END will show you the bottom

Close and save a file (CTRL + W)

CTRL + TAB will allow us to quickly switch between open documents

And SHIFT + C will collapse the feature manager at assembly level, if any structures or folders are expanded.

TAB at assembly level will quickly hide whatever the cursor is over, and SHIFT + TAB will bring them back

We can tile any open windows in a number of different ways, like vertically from the window menu

Using the G key (Magnifying glass) you can then select small faces without need to zoom in and out

Assembly

Copy with mates will allow us to duplicate the components and mates in multiple locations really quickly

There is a tool called “re-organise components” which can allow us to reposition components into different sub-assemblies, even if they are scattered all over your tree – we can select them graphically which makes life very simple.

If you are re-organising just by dragging in the feature tree – if you hold down CTRL it turns off the ability to drag into a sub-assembly.

Advanced select is another tool that can be used to quickly select components – by size for example – it is available from the S key shortcut menu, it’s the cursor symbol

If we want to be more specific, you could the select if toolbox option – which will ensure you only get toolbox components, perfect if you want to place them into their own folder

Assembly visualisation can help if you want to review properties each of the components have, for example “author” or “material” we can also sort by rebuild time, and graphical triangles – so if you are suffering from performance problems, this is a great place to start trying to figure out why.

You can save the selection as a colour coded display state for communication to others, or just for reference

Drawing

If we hold down shift on one of our views, we can move all of the views around as one

When creating a section view – hitting tab will change the type of section you are creating

On placing the view, if we hold down ctrl, it will break the alignment – and we can place it anywhere

The new section assist is great – but sometimes the section lines are a bit long, as it uses the bounding box of the model to work out the extents. We can right click on the sketch and edit it – then drag the lines closer to the model extents to tidying things up a bit

You can double click on a section line and it will reverse the direction

Half sections are a great way to display a model at drawing level

If we add a half section here, and then place the view – sometimes they are hard to understand as a user and even harder for a non-user.

You can use the 3d rotate tool to make sure you have everything in the correct orientation, but we can also save or use this in the current drawing.

The display is not ideal by default, but we change this by accessing the properties and changing the   cutting lines shoulders to not display (toggle box off)

At drawing level, you don’t need a BOM to use the balloon functionality – so we can add a balloon that is looking for the filename rather than a number.

We can also change the properties of the balloon and then apply the style changes to multiple entities

If we add a note, you can also ctrl + drag one of the points to create the next instance

Detail views can be any shape you like – they are not limited to circles and squares

Just sketch out spline – and then select the detail vie

You can double click on a section line and it will reverse the direction

Some people don’t want to show the detail circle around the area, or the perimeter around the view.

We can setup a custom “blank” layer style within the template, it needs to be A, -1, -1

You can then set the detail views to use this instead of the normal standard one

There is a fair amount to take in, and I would strongly urge you to watch the video, as a lot of the tips make more sense when shown in-context.

 

Innova Systems
We specialise in the supply, technical support and training of SOLIDWORKS software. Based in Cambridge we have a central location to service a UK wide customer base. We offer the skills and experience to help you develop new products using SOLIDWORKS - empowering smarter, faster and more cost effective design. We've been recognised by SOLIDWORKS Corporation for providing the highest rated customer support in Northern Europe in 2014, 2015 and 2016. Email: info@innova-systems.co.uk / Telephone: 01223 200690.
Innova Systems
Innova Systems
Innova Systems

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