Thank you this thread, I'm sure lots of posts will come rolling in.
1. I use them for any standard profiles that I do not want to make smart components, or features for. This can be as simple as a "standardized" slot that I may extrude cut or as complex as studying kinematics. Sometimes they are imported from legacy AutoCAD libraries. Sometimes they are a profile that I will use often within a single component or perhaps I will externally reference them throughout an assembly. Very useful things, these sketch blocks are... they are also all over my drawings too.
2. I wish linked sketch blocks didn't lose their relations when updated. Here's a nice thread:
3. The workflow isn't bad and doesn't appear to leave anything major to be desired other than the issue of losing sketch relations when updated. One minor annoyance when creating blocks is where the default origin may be, but typically it doesn't matter and is just annoying. Sometimes placing blocks within blocks can be a bit of a hassle, but again, nothing critical that otherwise cannot be done differently.
Thanks for the input guys, and yes I have seen that thread.
David, that message will appear if your block and the part you’re using it in have the same name. I will run this one by Development.
Regarding the disappearing relations, let me ask you another question. Let’s say you have a block in a part sketch, it’s a linked block, and has a tangent relation to some other entity in that part sketch. If you edit the original block file in its own window and remove the entity that has the relation, what would you expect to happen when you go back to the part sketch?
I’ll go ahead and tell you my initial thought on this, and that is to simply dangle the relation. If that were to happen, would you find this acceptable? Would you expect to see any behavior that may prevent you from getting into a dangling state?
Yea, I would expect that if I removed an entity that had an external relation that the relation would be lost as well (leaving it dangling would be nice so you would know it was lost and where). The thing that bothered me was that regardless of the change to the block, all relations were lost. The most egregious example I ran into is when you change a dimension inside a block. None of the entities have changed, their internal IDs should all remain the same, only a position has changed. And yet, all the relations it had are gone.
I used the Assembly Layout Sketch with Linked Blocks method on a very large, yearlong project, and as a result of this shortcoming, I have switched my method of top down design. I now use a “Sketch Part.sldprt” as my way to have multiple parts reference one file. Instead of an assembly with a layout sketch that parts relate to, I have an assembly with sub-assemblies that all contain the same “Sketch Part.sldprt” that the other part(s) in that sub-assembly relate to. Everything is mated coincident Front/Front, Top/Top & Right/Right so everybody is in the same place and mates don’t blow up when the internal ID of an element changes. I avoid “Convert Entities” like the plague and try to keep my relations between sketches rather than between a sketch and some other geometry whose internal ID potentially can/ usually will change. But I digress… If linked sketch blocks could work like my sketch part, I’d switch back in a minute. As you can see, my solution is a bit more arduous (although more stable).
As far as the error message goes, I named them the same so that I would know which block goes into which part. Seemed logical at the time... This is the only time I have seen a conflict between files that have the same name with different extensions. Definitely worth kicking up to Development.
In general I don’t produce drawings as my deliverables, so my exposure is limited, but I could see the high value of having properties update through blocks, and other AutoCAD like controls. The drawings functionality in general could use a healthy dose of enhancement (IMHO).
We use blocks in our sheet formats, for sections of the title block. The blocks are necessary to have certain text fields set with autocad attributes. But then, the "Define Title Block" feature is of no use because that tool can't deal with text fields in blocks.
We use blocks as groups of notes & lines in a drawing. Unfortunately you can't have properties update through the blocks - I had to create a new "object" that was two notes grouped together. I have a "North" arrow and "Travel" arrow that are blocks, approval blocks, logos, paint notes, etc. Lots of blocks for drawings.
I also use blocks when bringing in large sketches from ACAD. An example might be a car body and making it a block makes it a lot easier to deal with.
The sad part there is that ACAD handles those sketches with ease. SW chokes on them - big time.
Sketches in SW assembies (or parts) that contain blocks can create issues when the file is converted to an eDrawing file. The blocks tend to fly apart in the eDrawing- it seems to happen mostly with text entities. If I explode the same block then create the eDrawing, the same sketch will show correctly.
As now for creating block we insert model views (Part sketches are not enough to use as blocks)or isometric view in SolidWorks then creating their drawing and then save as DWG/DXF for creating blocks.
if it is possible to create block of model views directly( link will break of model and its convert the model edges as sketches) from drawing sheet then its reduce our work.
This is not often required but when required then work around is lengthy.
Good morning Robert,
After years of trying all kinds of different approaches, I still go back to how David Suelflow does it. I forget about blocks and assembly sketches, except in my nightmares of SW blow ups.
I have switched my method of top down design. I now use a “Sketch Part.sldprt” as my way to have multiple parts reference one file. Instead of an assembly with a layout sketch that parts relate to, I have an assembly with sub-assemblies that all contain the same “Sketch Part.sldprt” that the other part(s) in that sub-assembly relate to. Everything is mated coincident Front/Front, Top/Top & Right/Right so everybody is in the same place and mates don’t blow up when the internal ID of an element changes. I avoid “Convert Entities” like the plague and try to keep my relations between sketches rather than between a sketch and some other geometry whose internal ID potentially can/ usually will change. But I digress… If linked sketch blocks could work like my sketch part, I’d switch back in a minute. As you can see, my solution is a bit more arduous (although more stable).
I don't use blocks much. My primary usage is for sets of notes on drawings. This was particularly handy because we could group the text and the necessary boxes and ovals. I think this has been superseded by new and improved methods, but we still use the old blocks.
I've also used blocks to create repeated shapes, kind of like a derived sketch, where the same shape is required on a number of different features in a part.
First post in a long time but this frusterated me to the point I felt the need to post.
1. I use them for symbols, graphics, and in drawings (older and legacy tables). For instance I made 25 custom symbols from IEC 60878 last night for use in a design.
2. They only functionality you need to give them is to fix this relations issue and make RELATIONS TO THE ORIGIN!
3. Who cares about the workflow if blocks can't do the above.
If you use blocks in a skeleton part, and then insert the skeleton part into other parts..... changing the block in the skeleton part does not change the blocks in the subsequent parts. There is also no warning that anything is wrong, other than hitting control-q does not make the rebuild symbol go away. Opening and closing the subsequent parts makes the rebuild symbol go away, but the parts don't update. This limits blocks' usefulness in an area where they would be useful.
skeleton test.zip 437.1 KB
We use blocks for pneumatic schematics. Wish text could update without exploding or editing the block.
We also use blocks for positioning machine in a factory layout.
Block represent the machines from a plan view. The blocks are positioned relative to each other using dimensions. We the shift the dimensions to get the position of machines and conveyors where we need then.
Then as we model the machines we mate then machine assembly models to the plan view sketch.
Most of the time the plan view is in Autocad and we struggle combining it with the new layouts we are creating in SW.
Thanks everyone for the feedback. Noted on the limitations regarding relations and updates.
Tom, you mention your plan view is in AutoCAD most of the time. So all the blocks are initially created and positioned there first? If so, why not do the entire process in SolidWorks?
Also, you mention you wish notes would update without having to explode or edit the block. Would you also find it useful if you could update the geometry of the block without having to do either?
We use blocks to capture common hole pattern spacings or other common layout data in a complex assembly similar to a geodesic dome. This allows a common hole layout on things that are similar in family, but with subtle differences. Our CAD hardware is also a bit dated (WinXP 32bit). This helps reduce external references between components which keeps our assemblies behaving as they grow.
I learned of the "lost relations" deficiency after I had committed down the path of using the blocks. Made for a real pain.
I am finding a hard time finding information on blocks so hopefully you guys can help me!
My end goal here is to create a library of sketched block for slot and tab creation as well as some common bolt patterns we use. I would very much like to create my sketch using a design table but so far I have been unsuccessful in creating both the configured sketch and the block.
I am trying to copy a library system we already have for our fasteners. what you do is pick the type you want, drag it into your assembly and then a pop up window will allow you to select the appropriate size. this is what I want to happen when you drag the slot or tab block into your sketch. this process is what I can not find online. I have a feeling that I am going to have to create individual blocks for each size that I need. any input will be helpful here! thank you all in advance for you time.
PS we are using solidworks 2014 and headed into 2015 with in the next couple of months if that makes a difference.
A few thoughts...
-Slots in blocks - Seems cumbersome. When I tried this (using the Slot Sketch tool) I don't get the center Temporary Axis. May or may not matter to you.
-Slots are in the Hole Wizard now. You could look at setting up some Favorites - Hole Wizard Favorites is one of the File Locations so you can put it on a shared network location.
-For bolt patterns the basic function would work, dragging the block sketch from the Design Library, but I don't know a way to pop up a dialogue to change dimensions. There probably is a way with API or macros. The Configuration Publisher works like that - but it only comes up when you add a Configured part (or sub assembly) to an assembly.
-So I think you would have to edit the block to change dimensions. Or perhaps Explode the block - especially if you add more than one bolt pattern and want them to be different.
-For Fasteners are you talking about the SolidWorks Toolbox? Those are parts in any case - so similar thing can be done with Config Publisher.