Identify configuration-specific relations in sketch?

[Tom G]

I have an old repurposed design. I opened it this morning and checked its configurations before using it in a fab drawing. My intent was to manually update the cut lists in the weldment components for accurate parametric call outs in the fab. It had only one subconfiguration with the yellow error triangle, which wasn't present in its parent configuration. The two subconfigurations contain the same parts as the parent, but each with half of the components suppressed: to show an upper horizontal layout and a lower horizontal layout separately in views.

Note, I no longer do this in contemporary designs, but prefer Display States instead.

So I investigate one virtual contextual weldment component with the error, in the erroneous subconfiguration. The errors were in its 3D Sketch. As far as I can tell, it has the same relations and dimensions as it is used in other configurations. For some reason though, it is unsolvable and overdefined in this configuration only. Also, nothing was Dangling although it had suppressed related components. Also, the component does not fail, that is, it still populates the component with its weldments correctly.

I tried to use Display / Delete Relations to identify what to alter. I could not find any way to filter what is shown by configuration-specific relations. Is there such a way to identify and troubleshoot?

I'd rather not manually examine each and every relation in the sketch to see if something is selected to only apply here.
Don't suppressed relations in a sketch appear as greyed out? I could look for that in another configuration. Maybe I just answered my own query.

[Glenn Schroeder]

It's not a workflow I use, so I probably won't be able to answer any more questions about it, but if you right-click while in the open sketch and choose "Display/Delete Relations" from the drop-down you get the property manager shown below. As you can see, there are configuration options shown near the bottom.

image.png

[Rob]

Hi Tom

I have very occasionally used suppressed sketch relations.. they are tricky things.. The best way I found to manage them is via a Design Table

[matt]

Yeah, I avoid configurations. I know there are situations where they are difficult to avoid, but they cause all sorts of problems. Configuring sketch relations just sounds like asking for trouble. I'd rather swap out features than try to reuse one sketch with swapping relations. Configurations are just too easy to screw up, especially if you have multiple people working in the same files.

[Tom G]

Thanks guys. I'll take it on the chin for perpetuating an old design that carries old decisions with it.
In this case, somehow it errors but does not fail. For now, I'm merely living with the error.

[mike miller]

All good part files have errors. What's wrong?

[Glenn Schroeder]

Yeah, I avoid configurations. I know there are situations where they are difficult to avoid, but they cause all sorts of problems. Configuring sketch relations just sounds like asking for trouble. I'd rather swap out features than try to reuse one sketch with swapping relations. Configurations are just too easy to screw up, especially if you have multiple people working in the same files.

I use them, and for what I do I'd hate to have to do without them, but they can be tricky. Hardware is one of the places I use them most. I'd hate to think I had to have a separate Part file for every bolt size, type, and length. I use a lot of hex bolts, so for years I've had a single Part file for each diameter, with configurations for lengths. I didn't try to initially set up a configuration for every possible length, but just add them as needed. In addition to fewer files, this allows much easier edits if I need a bolt that's longer or shorter due to a design change. It's much easier to just switch configurations, which doesn't throw up errors, than to switch out a Part and then have to re-attach all the Mates.

I also have configurations for nuts and washers. Again, each size gets it's own file, but there are configurations for standard hex nut, heavy hex, coupling, jam, etc. For washers I have standard flat washers (F844), hardened washers (F436), and lock washers. (I made no attempt to make the lock washers with the offset, but I do have an extruded cut in them to show the cut. It's suppressed in the other configurations.)

[berg_lauritz]

Yeah, I avoid configurations. I know there are situations where they are difficult to avoid, but they cause all sorts of problems. Configuring sketch relations just sounds like asking for trouble. I'd rather swap out features than try to reuse one sketch with swapping relations. Configurations are just too easy to screw up, especially if you have multiple people working in the same files.

I use them, and for what I do I'd hate to have to do without them, but they can be tricky. Hardware is one of the places I use them most. I'd hate to think I had to have a separate Part file for every bolt size, type, and length. I use a lot of hex bolts, so for years I've had a single Part file for each diameter, with configurations for lengths. I didn't try to initially set up a configuration for every possible length, but just add them as needed. In addition to fewer files, this allows much easier edits if I need a bolt that's longer or shorter due to a design change. It's much easier to just switch configurations, which doesn't throw up errors, than to switch out a Part and then have to re-attach all the Mates.

I also have configurations for nuts and washers. Again, each size gets it's own file, but there are configurations for standard hex nut, heavy hex, coupling, jam, etc. For washers I have standard flat washers (F844), hardened washers (F436), and lock washers. (I made no attempt to make the lock washers with the offset, but I do have an extruded cut in them to show the cut. It's suppressed in the other configurations.)

I think, that having a single part file for nuts/washers etc. is valid, because the toolbox is just SO BAD. It just makes everything so much slower sadly.

The only VERY new tool I found, that changed my mind is this one:
https://cadbooster.com/solidworks-add-i ... er-filter/
I couldn't convince my supervisor, but I was hooked, when I tried it.

We also do configurations on parts where we only change one dimension and the configurations are named like this: [part#]-[length]

Same issue here: performance takes a hit.

[Tom G]

Hi Tom

I have very occasionally used suppressed sketch relations.. they are tricky things.. The best way I found to manage them is via a Design Table

@Rob - Great idea! This assembly did not already have one, so I auto-formed it.
Insert -> Table -> Design Table -> Auto create
This allowed it to identify everything different between configurations.
I searched for a unique word in the name of the faulty component, and it was only found in STATUS for being resolved in the arrangement configurations and suppressed in the fab configurations, as intended. This at least narrowed it down for me that the error is NOT a suppressed relation or config-specific relation.
In a more granular fashion, I could repeat this within components as well.
Thanks!

+1 Correct answer to Rob (heh)

[Frederick_Law]

Yeah, I avoid configurations.

Use config with suppress feature.
Easier to manage since you can see what's happening.

[DennisD]

I use configurations A LOT. Most of my work is in R&D so it makes sense. The part configurations represent different design iterations/ideas. Assembly configs make it a simple thing to compare different versions side-by-side. Often I'll make a top level assembly with a linear array of one or more subassemblies in development. I really like how easy it is to make the instances of the array use a different configuration. I also use assembly configs for different stages of mechanical components, such as cylinders or springs: Retracted/Compressed, Extended/Uninstalled (or Uncompressed), and Range of Motion.

I usually take my configurations to a Design Table very quickly. I much prefer the ease of the Excel logic over the Equation Editor, plus color coding, referencing other worksheets, etc., make DT's a great workspace.

I ALWAYS name my features upon creation, whether the part will have configurations or not. And I ALWAYS name the dimensions (and sometimes sketches) that will be used in a configuration. This makes using the Design Table so much clearer.

[mattpeneguy]

Tom,
Can you post this part? I'd like to take a look at it...Though, there's probably IP involved, or you would've done that already I'm guessing?

[Tom G]

@mattpeneguy It is a conjoined tubing drain across the entire piping system, virtual and in context. I'd have to share the entire work, so yeah, IP. It's 3D Sketch in question is comprised of tangent lines and arcs, and mysteriously fails only in one subconfig which is utilized for only one view in one drawing document that has already been finalized. I'm overlooking it b/c it doesn't affect production data at this point.

I do admit that this may be a poor 1st example on this new forum for How to Ask a Good Question. Not even an image attached. Sorry. Next monkey can do better.

[Merovingien]

sometimes to "help" a "3D-sketch" too complexe
you can use (partial-use) some "2D-sketch"
like to sub-dividing it...

sometimes in 3D-sketch, removing X, Y, or Z colinear to some line, and replace it by "paralal to a base-plane" can help.