Have you ever tried bringing a DXF or DWG file into SOLIDWORKS?
If not, it's just "File, Open" to do this - set your file type to "All" or the specific type you are looking for,
select the file and hit "Open" - you will then get this window: -
Generally, you want the options to import to a new part, as a 2D sketch.
When you hit "Finish" you will find yourself editing a completely undefined sketch.
This is OK, if the DXF/DWG was of a nice simple engineered part - you can add relations and dimensions manually
or possibly use the right-click short-cut to "Fully Define Sketch."
But, something stylized like a logo will have some areas with splines, and other areas with lines and arcs, and you can't change the shape at all. Particularly if it is a trademarked logo - otherwise the trademark will not apply.
So, if you need to resize the logo or rotate it, you can be struggling.
The answer is to save the sketch as a block.
You can stay in the sketch, editing it - go to Tools, Blocks, Make...
Then select any sketch geometry that you want to be part of your block - you can window select it if you like.
Notice what looks like a large blue origin in the picture above - this is the "Insertion Point" - it appears on
screen if you expand the left hand panel section by the same name.
This is where your cursor will be when you insert the block into any other file - one of the benefits of having your logo (or your customer's logo) as a block.
Drag it to somewhere sensible relative to your geometry, then hit the green tick.
The geometry on screen will then go grey - as if you are not editing the sketch any more - but you are...
The geometry is now a block - one single rigid entity.
You will see that there is now a block listed on the design tree - embedded into the sketch.
If you right-click the block you will get the option "Save Block" - this will enable you to use that same block in any SOLIDWORKS files in the future.
Now, when you are creating your sign - or any other part where you want to have a physical version of that logo,
you can create a sketch and then go to Tools, Block, Insert - then browse to your block file, select it and hit "Open."
After placing the block into your sketch, shut down the "Insert Block" command, and you will find that if you click on the block, you can scale it or rotate it using the options on the left.
If you drag it, it will move as one thing - which was the point really!
You can of course use sketch relations and/or dimensions to position it.
When you are happy, create your cut or extrusion feature, apply a colour or appearance to it - and there you go: -
I hope that helps!