Back in February we posted an article about how to cut back on the time you spend sketching, particularly when you find yourself sketching the same type of geometry multiple times. In the Tech Tip titled Reduce, Reuse, Recycle Your Sketches, I discussed two of the three techniques you can use to avoid spending time recreating sketches you’ve already made, whether that be within the same part or a different one. We discussed copying and pasting sketches, as well as creating derived sketches. Today I will discuss the third technique: Sketch Blocks.
Sketch blocks in SolidWorks can be very powerful. I will walk you through the process of creating a block and then inserting it into a new part. I will then show you how to designate whether the inserted block remains linked to the original block file so that it updates when the original final is changed. Finally I will discuss other uses of blocks that don’t necessarily contribute to a library of sketches, but can be just as beneficial.
You can access your sketch block tools by going to Tools > Blocks or by activating your Blocks menu. To do this, right click over the CommandManager at the top of your SolidWorks window, and chose the “Blocks” menu. There are several icons that this will place on your workspace. If you open a blank part file and look at this menu, the only available option is to insert a block. Most of the block tools you will use from the sketch environment.
1. To create a sketch block, first open a part and create a sketch. This does not necessarily need to be a blank part, you can create and capture a sketch block from a part that is partially or fully modeled.
2. The next step is to sketch the entities that you would like to be a part of the block. Again, if you’ve already captured this in a sketch, simply open that sketch for editing so that the individual entities are selectable.
3. At this point you can either chose to “Make Block” 
or “Save Block” 
. If you want to include all entities in the sketch in the block, you can use “Save Block”, which will save the entire sketch as a .SLDBLK file. You should chose to save this block somewhere you will remember in the future. By going to Tools > Options > System Options > File Locations, you can designate a location on your computer to automatically save and search for blocks.
4. If you choose to “Make Block” you can select certain entities to be part of the block and exclude others.
a. Using “Make Block” you also can create an insertion point. By dragging the blue insertion icon around, you can snap it to geometry in the block. Then when you insert this block in a new part, you can control where the block is placed based on this point.
b. Once you make a block, it will show up in your feature tree embedded inside the sketch you created. The sketch entities will also turn gray. This block is not yet available outside the part you are currently working in. You still need to Right click on this block in the feature tree and choose “Save Block”. This might seem like a longer process than simply choosing “Save Block”, as in step 3, however, as I eluded to earlier, there are more things that can be done with Blocks, in which making a block without saving it can be helpful.
5. Now that you’ve created and saved a block, it is very easy to use that block in a new part:
a. Simply open the part in which you’d like to insert the new block and go to Tools > Blocks > Insert Block or select the “Insert Block” 
icon from the Blocks menu.
b. At this point, if you haven’t already done so, you will be instructed to select a face or plane for the block to be placed on. A new sketch will be opened on that face/plane and the block will appear attached to your mouse (at the location of the insertion point if you have specified one).
c. Place the block wherever you’d like. You can place multiple in the same sketch.
6. If you click on any entity within the sketch you can see the block properties on the left side of the window. Within this property manager you can choose whether or not this block is linked to the original block file. The main benefit to linking your blocks is to ensure that the block will update in all parts where it is used. If you have “Link to File” unchecked, you can choose from here to edit the block or assign a new insertion point. If “Link to File” is checked, you do not see these options because the block can only be edited by opening the original .SLDBLK file.
7. In the Parameters section of the Block properties manager you can scale or rotate the block. If you check the box that says “Lock Angle” the angular orientation of the block will be locked and cannot be adjusted unless the box is unchecked.
8. One more thing you can chose to do with a block once it has been created is explode the block 
. This will dissolved the block back into regular sketch entities. If you exploded a block that was linked to a .SLDBLK file, this will automatically break that link. If you explode a block that has been scaled, you will notice that all dimensions within that block are now scaled appropriately.
One more way blocks can be used in a very convenient manner is simply to lock a set of entities together temporarily for the purpose of moving them as a unit without worrying about these entities moving or shifting in respect to one another. This is a simple way to set up a 2-D schematic in SolidWorks. You can also repeatedly insert these blocks that ARE NOT saved externally, as long as it is within the same part.
If you use “Make Block” to group sketch entities together, you may notice SolidWorks creates this block in the feature tree as Block1-1 for the first block, Block2-1 for the second, etc. You can rename these blocks, but they will maintain the “-1” at the end of the name. You can chose “Insert Block” and the blocks that already exist in that part are available to be inserted. Once you insert new versions of the same block you may notice the name of the new Block in the feature tree is the same as the original, but with a “-2” or “-3” following instead of “-1”. You can also link, scale, rotate and explode this block, just as you can with the externally saved .SLDBLK files.
At this point, we’ve discussed creating, saving, and inserting blocks. These are all the tools you need to build an arsenal of predefined sketches that can be re-used as many times as you’d like, without the need to hunt down the original part where the sketch existed. By exploding blocks you can then take advantage of the convenience of working from a normal sketch, without needing to build that sketch from scratch. Sketch blocks are available in the part, assembly and drawing environment, making them extremely flexible. I’ve hopefully shown you that from now on there is no need to repeat the same boring sketches over and over; you could be spending less time sketching and more time on the more important aspects of your design.
Hitchhiker’s Guide to Upgrading your SolidWorks Environment to 2013
We’re past the final day of the Mesoamerican Long Count calendar… That means life will, indeed continue. Are you prepared? If not, join us for a Hitchhiker’s Guide to Upgrading your SolidWorks Environment to 2013!
