SOLIDWORKS Tips & Tricks

[AD Design]

SW Index

Thanks for posting this len_1962, will be looking through this later

 

[ChipSplitter]

Here's another gem from the SW forum.

My collection of tips, tricks and best practices. | SOLIDWORKS Forums

Lots of best practice advice as well as tips and shortcuts. Kudos to Henk de Bruijn.

Not me, BTW.....

 

[MasterJack]

Great thread - just thought I would add a few...
1. Use Derived Sketches if you need to use the same sketch on different planes / surfaces.
2. Use Assembly Visualization to populate custom properties. A BOM can also be used. Files need to be checked out for it to save the information.
3. You can draw a line and start with an angle – choose the angle on the left pane.
4. This tip works anywhere in Windows: If you are going to paste something you copied, use Windows-Key-V and it will let you select from everything you have copied to the clipboard since your last reboot. Very handy.
5. You can create a new part similar to another by using MAKE INDEPENDENT. Useful if you want to use an existing bolt (for example) and save it under a new name. This would replace opening an existing bolt, doing a save-as-copy, giving it a new name, then modifying it.
6. If you modify a sketch such as to change it’s shape, don’t delete entities, convert them to construction so it will not break any sketch relations. You can also delete an entitiy and REPLACE it with a new one so sketches don’t break.
7. You can use VIRTUAL COMPONENTS within an assembly to save the part ONLY IN THE ASSEMBLY – no external component will be created. Good for Misc parts that need to be in the BOM but do not have a part number. One advantage is if you make all of your parts VIRTUAL, you can send your assembly to a client without the need to send all the parts along with it. All parts would be contained in the assembly.
8. In drawings – you can pre-select multiple edges, then create a note and you will have arrows pointing to all edges.
9. If you decide you don’t want a component in the BOM, you can of course EXCLUDE FROM BOM in the assembly, but if you want to delete the entire row – FIRST drag that part (in the BOM) to the very bottom, then delete it – that way your numbering does not get messed up.
10. Use INTERSECT feature to create an internal body (for example – the water in a bottle). Select plane that cuts through the body and select the body, then INTERSECT. Click on Create Internal Regions, hit checkmark. Do not merge result. You will end up with 2 halts, merge them using Combine.

Just a few to get started...

Thanks,

John

 

[Halcyon]

Name variables as you make sketches and dimension stuff. Instead of typing in "1" for a hole dia, type something like "holedia=1", and now you can utilize the variable "holedia" later on. Want to place the hole so the centerline is 3/4 of a diameter away? Just dimension that feature and type in "=holedia*0.75", and it will maintain that, even if you change the parameter. You can also do crazy stuff like trig equations and more.

You can do it with feature patterns too. Want to pattern say, 5 holes on a 5" piece of stock? Do something like 'rectanglelength/holecount'(you'll have to make sure those parameters exist in your file). Define the 'holecount' parameter as 5. Then when you do your rectangular pattern, call up that same 'holecount' parameter. Now if you change that parameter it not only updates the original hole placement, but the concurrent patterned ones as well. I try to use parameters as much as humanly possible when drafting stuff because they really make life easy. Although I usually shorthand stuff for efficiency, so I'd call it something like 'rectw' and 'holect'. Parameters are great though.

 

[BRHMFG]

Great thread! Is there a way to export dxf from a face in SW in a single click? Often I need a simple plate in the shop and I've never counted the clicks it takes to take a simple part from SW to CNC plasma but its a lot (if I include running it through nesting). I could theoretically draw the part at the machine but like to run it through nesting so all speeds and gas setting are done for me.
So in SW I select face, Save as DXF (1) brings up left dialogue box, click OK (2) brings up my layer mapping, hit ok (3), brings up the preview (4) finally its saved. I know its minor but is there a shortcut? Can I make a button for it?

 

[Halcyon]

Great thread! Is there a way to export dxf from a face in SW in a single click? Often I need a simple plate in the shop and I've never counted the clicks it takes to take a simple part from SW to CNC plasma but its a lot (if I include running it through nesting). I could theoretically draw the part at the machine but like to run it through nesting so all speeds and gas setting are done for me.
So in SW I select face, Save as DXF (1) brings up left dialogue box, click OK (2) brings up my layer mapping, hit ok (3), brings up the preview (4) finally its saved. I know its minor but is there a shortcut? Can I make a button for it?

You might be able to achieve that using macros.

Record Macro:

Record SOLIDWORKS Macro - 2022 - SOLIDWORKS API Help

help.solidworks.com

Map macro to button:

Assign SOLIDWORKS Macro to Button - 2022 - SOLIDWORKS API Help

help.solidworks.com

 

[rcoope]

Great thread! Is there a way to export dxf from a face in SW in a single click? Often I need a simple plate in the shop and I've never counted the clicks it takes to take a simple part from SW to CNC plasma but its a lot (if I include running it through nesting). I could theoretically draw the part at the machine but like to run it through nesting so all speeds and gas setting are done for me.
So in SW I select face, Save as DXF (1) brings up left dialogue box, click OK (2) brings up my layer mapping, hit ok (3), brings up the preview (4) finally its saved. I know its minor but is there a shortcut? Can I make a button for it?

Yes you can just Save-As, pick DXF and it lets you select the face you want to save. I usually square up to the face and then Save-As so I'm sure I have it right.

 

[kinetiq]

Great thread! Is there a way to export dxf from a face in SW in a single click? Often I need a simple plate in the shop and I've never counted the clicks it takes to take a simple part from SW to CNC plasma but its a lot (if I include running it through nesting). I could theoretically draw the part at the machine but like to run it through nesting so all speeds and gas setting are done for me.
So in SW I select face, Save as DXF (1) brings up left dialogue box, click OK (2) brings up my layer mapping, hit ok (3), brings up the preview (4) finally its saved. I know its minor but is there a shortcut? Can I make a button for it?

Right-click Face, type "X" (Export to DXF / DWG), type Filename, <enter> to close dialog, <enter> to confirm export.

That's pretty dang quick.