CAD Forum

[/rant]

Ok, I feel a bit better now.

FYI, SE doesn't do this, and it's so much better for it.

Can you be a bit more specific with examples..? Maybe I can be of help

AlexLachance wrote: ↑Tue Jun 07, 2022 10:43 am Can you be a bit more specific with examples..? Maybe I can be of help

Its a difference in behavior and I can see pros and cons to both.

• SolidWorks, suppressing a feature will also suppress downstream features that rely on it.
• Solid Edge, suppressing a feature, does suppress downstream features, it leaves them in on in the tree with errors.

AlexLachance wrote: ↑Tue Jun 07, 2022 10:43 am Can you be a bit more specific with examples..? Maybe I can be of help

Oh, it's just a rant, but the tags don't work on an image I guess.

I've asked all over and apparently there's no way to turn off the "feature" of Solidworks suppressing downstream features when I suppress one upstream feature but just leaves them suppressed. It wreaks havoc on an old process I used regularly in Solid Edge, and I have not yet blead it from my habits. So out of instinct I'll suppress one thing up stream intentionally to see what's affected but then all dependents are suppressed but unsurprising it still leaves all those other features suppressed. So now I have to go unsuppressed them all, if I already had some features suppressed there's no telling them apart. It's not so bad on my own models, but if trying to understand someone else's it's tougher. Then if some features are configured and suppressed for that reason I really screw things up. It's just very unhelpful behavior IMO. But maybe I'm just modeling wrong...

I feel your pain. I've often fought trying to find the dependency so I can delete a feature that's no longer needed.

For years people have been asking for the software to show errors instead of suppressing (or deleting) downstream features when another feature is deleted or suppressed, but it hasn't happened yet. Hopefully it will before I retire.

bnemec wrote: ↑Tue Jun 07, 2022 10:53 am It's not so bad on my own models, but if trying to understand someone else's it's tougher. Then if some features are configured and suppressed for that reason I really screw things up. It's just very unhelpful behavior IMO. But maybe I'm just modeling wrong...

I can think of a few cases where I would like the SE option. For interrogating the models, you have the parent/child indicators to see what's affected.

jcapriotti wrote: ↑Tue Jun 07, 2022 10:48 am Its a difference in behavior and I can see pros and cons to both.

• SolidWorks, suppressing a feature will also suppress downstream features that rely on it.
• Solid Edge, suppressing a feature, does not suppress downstream features, it leaves them in on in the tree with errors.

FIFY, unless they've changed something.

The big difference is, in SE when that parent feature is unsuppressed the rest of the features rebuild, in SW they stay suppressed. I don't understand why people think a failed feature is catastrophic. It's history based modeling, actually it's really high level sequential programming language. Change something upstream and down stream likely to fail, sometimes it's very simple/fast to fix them sometimes its not. That's the whole process in how I understand it.

bnemec wrote: ↑Tue Jun 07, 2022 10:53 am Oh, it's just a rant, but the tags don't work on an image I guess.

I've asked all over and apparently there's no way to turn off the "feature" of Solidworks suppressing downstream features when I suppress one upstream feature but just leaves them suppressed. It wreaks havoc on an old process I used regularly in Solid Edge, and I have not yet blead it from my habits. So out of instinct I'll suppress one thing up stream intentionally to see what's affected but then all dependents are suppressed but unsurprising it still leaves all those other features suppressed. So now I have to go unsuppressed them all, if I already had some features suppressed there's no telling them apart. It's not so bad on my own models, but if trying to understand someone else's it's tougher. Then if some features are configured and suppressed for that reason I really screw things up. It's just very unhelpful behavior IMO. But maybe I'm just modeling wrong...

Yes there is, it's just very unconventional.

Now that you've suppressed your feature and that the other features have been suppressed, you can note the suppressed feature, undo the process and then go into these features that were suppressed and figure out what is causing them to be suppressed to correct this.

In SolidEdge. You supress the feature, and then go into these features with errors and correct these errors.

In SolidWorks, you can supress the feature, note the undesirably suppressed feature, undo the process, go back to correct what's necessary in these features, and then and only then can you supress your feature so that your underlying features will not be supressed.

I guess it's a matter of what you're used to. I'd rather keep the links, when needed, and correct the unnecessary links, so that the file can be a valid "startup file" for the future.

jcapriotti wrote: ↑Tue Jun 07, 2022 10:57 am I can think of a few cases where I would like the SE option. For interrogating the models, you have the parent/child indicators to see what's affected.

image.png

Those only go one level, need daisy-chained/recursive indicators. That's why I use the "suppress and see" method that, I thought worked very well and fast in Edge. I just got to get over the SW behavior, but gol-dang-it, it's extra functionality that's not desired. I just want to turn that part off! Just let the features fail, I'll either unsuppress the parent feature or fix it and they rebuild. Often, it's just one or two little things at the second or third level and all the rest rebuild.

AlexLachance wrote: ↑Tue Jun 07, 2022 11:01 am
In SolidEdge. You supress the feature, and then go into these features with errors and correct these errors.

I believe NX behaves the same way as SE.

bnemec wrote: ↑Tue Jun 07, 2022 10:29 am
image.png


Ok, I feel a bit better now.

FYI, SE doesn't do this, and it's so much better for it.

I loathe other features from SE too:
Synchronous modeling i.e.

How about we make a workflow that 'copies' it?

Example (what we are currently ALMOST doing):

• Import geometry (1 feature)
• Modify however you like, use whatever feature
• put it back into only bodies (I requested a macro for this and it's nice for simplifying a modified model)
• keep body/face/edge/vertex IDs (not implemented into the macro but should be possible, right? And then SWX would keep the mates? One can dream...)
• because it's imported you can now use feature recognition for things you might want to adjust (i.e. hole wizard etc.)
• use another macro to fix/unfix the sketch you're trying to modify (leave sketches basically unconstrained most of the time)
• feature tree now only has an imported body plus some features you converted/added in there

It wouldn't be perfect but it's something!

And in the consistently inconsistent department. Suppressing a "seed" component in SW does not suppress patterns based on that component. That is one case where I wish it would.

AlexLachance wrote: ↑Tue Jun 07, 2022 11:01 am Yes there is, it's just very unconventional.

Now that you've suppressed your feature and that the other features have been suppressed, you can note the suppressed feature, undo the process and then go into these features that were suppressed and figure out what is causing them to be suppressed to correct this.

In SolidEdge. You supress the feature, and then go into these features with errors and correct these errors.

In SolidWorks, you can supress the feature, note the undesirably suppressed feature, undo the process, go back to correct what's necessary in these features, and then and only then can you supress your feature so that your underlying features will not be supressed.

I guess it's a matter of what you're used to. I'd rather keep the links, when needed, and correct the unnecessary links, so that the file can be a valid "startup file" for the future.

I don't think we're talking the same thing here. What you're suggesting is very much more tedious and slow than toggling a feature off and back on in SE. Much of the time I did it to learn how the model was made, not that I was actually going to delete the feature.

Add this button to your right click or a toolbar. Needs to be there by default IMO. Command has been there since the beginning but it was only accessible under the "edit" menu until they allowed customizing the right click menu.

jcapriotti wrote: ↑Tue Jun 07, 2022 11:09 am Add this button to your right click or a toolbar. Needs to be there by default IMO. Command has been there since the beginning but it was only accessible under the "edit" menu until they allowed customizing the right click menu.

image.png

most impressive trick in a while!

bnemec wrote: ↑Tue Jun 07, 2022 11:06 am I don't think we're talking the same thing here. What you're suggesting is very much more tedious and slow than toggling a feature off and back on in SE.

Yes, indeed, but if the suppression of the feature happens, it is because there is a relation to it.

Is the relation Required? If yes, then keep it.
If no, then remove it and if it needs to remain, have it independant from whatever feature it was in.

bnemec wrote: ↑Tue Jun 07, 2022 11:06 am Much of the time I did it to learn how the model was made, not that I was actually going to delete the feature.

How is that different then..? You're basically learning how the model is made with the process I spoke of, it's a lot more tedious, that I can agree, but that's only for now.

It becomes less tedious with time until it becomes instinctive to "know" how to build things without creating useless parent links.

The parent child indicators are the way to go to see what's related. NX has color coding where you select a feature in the tree and upstream are one color and downstream are another. SE does this but you have to right click and select it.

After my 4 years on NX a long time ago, I hounded the hell out of SolidWorks to add this, alpha tested it for them, and we finally got it a while back.

jcapriotti wrote: ↑Tue Jun 07, 2022 11:27 am The parent child indicators are the way to go to see what's related. NX has color coding where you select a feature in the tree and upstream are one color and downstream are another. SE does this but you have to right click and select it.

After my 4 years on NX a long time ago, I hounded the hell out of SolidWorks to add this, alpha tested it for them, and we finally got it a while back.

Again, Parent Child indicators only go one layer in SW. I have them on and use them most of the time. Although I don't understand why they don't stay turned on, like they're a doc setting not a system setting.

AlexLachance wrote: ↑Tue Jun 07, 2022 11:13 am Yes, indeed, but if the suppression of the feature happens, it is because there is a relation to it.

Is the relation Required? If yes, then keep it.
If no, then remove it and if it needs to remain, have it independant from whatever feature it was in.

How is that different then..? You're basically learning how the model is made with the process I spoke of, it's a lot more tedious, that I can agree, but that's only for now.

It becomes less tedious with time until it becomes instinctive to "know" how to build things without creating useless parent links.

It sounds like you haven't toggled parent features suppressed on off in Solid Edge?

bnemec wrote: ↑Tue Jun 07, 2022 11:33 am It sounds like you haven't toggled parent features suppressed on off in Solid Edge?

I've never actually worked with SolidEdge more then an hour, but I don't really see a difference between
-Supressing a feature and correcting the errors
-Removing useless parent relations in features so that only the desired feature gets supressed when supressing.

I've worked with SolidWorks and AutoCAD, done a bit of SolidEdge at home and also a bit of Inventor, but I wouldn't be able to help anyone relating SolidEdge/Inventor.

Perhaps you need to rethink the order of your features..?

In Creo (Pro/e) you can do this by "Suspending".
Agree, I get so frustrated with the parent/child illogical nonsense SolidWorks applies.
Here SW Corp, call it "STEPCHILD" Send that word to your marketing dept and tell the to sit and spin!

Wasn't this one of the Top Ten list items for 2022?

HDS wrote: ↑Tue Jun 07, 2022 12:39 pm Wasn't this one of the Top Ten list items for 2022?

Yes. It was even voted #1. See https://www.engineersrule.com/the-resul ... orld-2022/. It was one of several good ones submitted by @Alin.

There is a very old tool in NX called Feature Playback- as I recall it might be called just "Replay" now. It sounds like its name. It's a player control that allows you to step through or forward to or rewind to specific features to understand how the model was built. The nice thing about this tool is that you can go directly to the edit function (normally the same creation dialog of that feature) of that feature during the replay and continue to make multiple edits throughout the replay.

Ry-guy wrote: ↑Tue Jun 21, 2022 3:44 pm There is a very old tool in NX called Feature Playback- as I recall it might be called just "Replay" now. It sounds like its name. It's a player control that allows you to step through or forward to or rewind to specific features to understand how the model was built. The nice thing about this tool is that you can go directly to the edit function (normally the same creation dialog of that feature) of that feature during the replay and continue to make multiple edits throughout the replay.

SolidWorks 'rollsback' when editing sketches and features, so I believe it works in a very similar way to the tool you are refering to. His issue is more or less that features get suppressed rather then losing whatever reference it was that was linked to whatever other feature that was originally suppressed above it.

Example:
Solidorks: Create an extrude and then cut through it. The cut is dependant of the extrude. If you supress the extrude, the cut gets suppressed.

That other program : Create an extrude and then cut through it. The cut is dependant of the extrude still. If you supress the extrude, the cut remains active but pops an error because it's missing it's reference.

Ry-guy wrote: ↑Tue Jun 21, 2022 3:44 pm There is a very old tool in NX called Feature Playback- as I recall it might be called just "Replay" now. It sounds like its name. It's a player control that allows you to step through or forward to or rewind to specific features to understand how the model was built. The nice thing about this tool is that you can go directly to the edit function (normally the same creation dialog of that feature) of that feature during the replay and continue to make multiple edits throughout the replay.

Edge has it too IIRC, and I miss it. I forgot how to get to it but I used it fairly regularly when opening someone else's model (and my own that I haven't touched in a few months).

SW will let user suppress parent features, but instead of lighting up the tree with failed dependents it will suppress all the dependents all the way down the tree. Fine, but when I unsuppressed the parent it leaves all the dependents suppressed which is a huge PITA IMO. Deleting a parent does the same thing, except it will usually delete the dependents. It completely undermines my old method of familiarizing myself with the model; suppress feature, see what fails, unsuppress the parent and investigate the children. I'm moving on I just don't suppress features in the feature tree.

I really miss that feature in NX.

bnemec wrote: ↑Tue Jun 21, 2022 5:06 pm Edge has it too IIRC, and I miss it. I forgot how to get to it but I used it fairly regularly when opening someone else's model (and my own that I haven't touched in a few months).

SW will let user suppress parent features, but instead of lighting up the tree with failed dependents it will suppress all the dependents all the way down the tree. Fine, but when I unsuppressed the parent it leaves all the dependents suppressed which is a huge PITA IMO. Deleting a parent does the same thing, except it will usually delete the dependents. It completely undermines my old method of familiarizing myself with the model; suppress feature, see what fails, unsuppress the parent and investigate the children. I'm moving on I just don't suppress features in the feature tree.

Little suggestion. Use undo rather then unsupress.

Undo will bring the child features back to unsupressed.

Unsupress won't unsupress the child features, because the feature you are unsuppressing does not require those features to generate itself. You could unsupress the lowest feature and it would most likely do the result you desire too.

I know it doesn't sound logical to you, but it's logical in terms of operation for the program and programming.

AlexLachance wrote: ↑Wed Jun 22, 2022 11:07 am Little suggestion. Use undo rather then unsupress.

Undo will bring the child features back to unsupressed.

Unsupress won't unsupress the child features, because the feature you are unsuppressing does not require those features to generate itself. You could unsupress the lowest feature and it would most likely do the result you desire too.

I know it doesn't sound logical to you, but it's logical in terms of operation for the program and programming.

Alex, respectfully, I think you'd just have to use Solid Ege history based modeling for a while to get where I'm coming from on this. I think I have a decent 30,000ft grasp of feature dependency, that's not the problem here it's just the bad UI IMO.

Also, SW has already trained me to not rely on undo/redo. I would say never rely on undo, but sometimes it does what I expect, sometimes it does not. Since I have not discovered the algorithm to how undo and redo function in SW I just avoid them mostly. I expect over time I will slowly get more comfortable with it as my memory charts the pitfalls.
Edit: I'm going to make a conscious effort to use undo after I suppress a feature I should not have.

bnemec wrote: ↑Tue Jun 21, 2022 5:06 pm Edge has it too IIRC, and I miss it. I forgot how to get to it but I used it fairly regularly when opening someone else's model (and my own that I haven't touched in a few months).

SW will let user suppress parent features, but instead of lighting up the tree with failed dependents it will suppress all the dependents all the way down the tree. Fine, but when I unsuppressed the parent it leaves all the dependents suppressed which is a huge PITA IMO. Deleting a parent does the same thing, except it will usually delete the dependents. It completely undermines my old method of familiarizing myself with the model; suppress feature, see what fails, unsuppress the parent and investigate the children. I'm moving on I just don't suppress features in the feature tree.

@jcapriotti mentioned that you can 'unsuppress with dependants' in a different thread. Use that! It's like magic and one of my favourites!

berg_lauritz wrote: ↑Wed Jun 22, 2022 11:34 am @jcapriotti mentioned that you can 'unsuppress with dependants' in a different thread. Use that! It's like magic and one of my favourites!
2022-06-22 10_34_23-SOLIDWORKS 2021 SP4.1 - [B080646.SLDPRT _ [Read-only]].png

That's even better, let's hope SolidWorks doesn't break it soon

Did some test on this topic on this brain dead design tool.

Just draw a box and add a cutout.
Then fill in the cutout with a boss using convert entities from the cut-extrude1

Then suppress the added feature.

The we add another boss with using convert entities from the hole.
So lest try to unsuppress the Boss-Extrude7
We gets some errors as the included reference from the cutout is now gone.
Maybe its was a mistake so we supress the Boss-Extrude7 again.


But as we can see the error still exists. Pressing the stupid traffic light will not fix it.
The only way to fix it is to press ctrl+q.


If we then compare it with a tool that actually is helping the end user to investigate he/her ideas.
So what will happen when we unsuppress protrusion 2 which will fill in the cutout, the same as in shitty SW ?
No error at all.
So what's happen here ?
Lets lock at the last Protrusion 3 sketch .
It sort of remember its reference. In other words it will gladly follow what end user want to do and not force its own stupid rule set on what is allowed.

Its amazing how broken this SW really is.

In a similar vein, I hate that Solidworks won't let me do many things I want to do because it thinks it knows better. I can't move a child feature above the parent. I can't create a sheet metal flange with errors. I can't delete all the features and sketches I want to delete in one command.

Dwight

Dwight wrote: ↑Mon Mar 11, 2024 1:19 pm I can't move a child feature above the parent.
Dwight

So you want the child born before the parent?

this is probably the reason I often find some model with like 20% of the tree suppresed. the engineer probably tried to disable the feature suppressing it, sort of trying to delete before deleting for real, but in the end nothing were deleted leaving the model in a less then desiderable shape and nobody knows why the suppression happened In the first place...

to undo suppression on children I just shift select the whole tree and unsuppress from the edit menu.
not the best, but at least there are not remains of unwanted suppression around. And we do not use configurations in parts so suppression should not be used in our part models.

Frederick_Law wrote: ↑Mon Mar 11, 2024 2:17 pm So you want the child born before the parent?

I cannot speak for Dwight, but what you say is one of the uses. Maybe didn't bother to check refs or aware of the ref, but not obvious why there's a ref, some people's sketches get crazy or could be feature parameters. Either way, allowing the user to put the child before the parent with failed feature/sketch etc makes finding the refs very simple to identify. Then user can quickly determine if the child really is a child of the parent or it was just sloppy sketching/modeling that should be cleaned up. People forget you can do time travel in history based modeling; go back in time and right the wrongs.

Put reference in sketches.
Don't project/convert from model.
Reuse the sketch.
Features can move up and down.
Just not above the sketch.

Frederick_Law wrote: ↑Mon Mar 11, 2024 4:30 pm Put reference in sketches.
Don't project/convert from model.
Reuse the sketch.
Features can move up and down.
Just not above the sketch.

Preach on! But you know, the out of box training shows how to use the software. Not always so much how to use it properly, usually focus on what it can do and speed. So people all model for speed not paying attention to what sketch elements are snapping to.

The ability to see what fails after suppressing something that happens to be a parent or reording child before parent is a great teaching tool to get people to model more robustly as you suggest. It shows them what they did wrong, often they don't even notice all the bad sketch relations. Solidworks' method of just suppressing the features or blocking actions that would fail features teaches them to either leave all the suppressed features for the next person or delete them and make new. Or even worse, instead of editing features to make the change(s) they just slap more and more features on the end of the tree.

bnemec wrote: ↑Mon Mar 11, 2024 4:47 pm Preach on! But you know, the out of box training shows how to use the software. Not always so much how to use it properly, usually focus on what it can do and speed. So people all model for speed not paying attention to what sketch elements are snapping to.

The ability to see what fails after suppressing something that happens to be a parent or reording child before parent is a great teaching tool to get people to model more robustly as you suggest. It shows them what they did wrong, often they don't even notice all the bad sketch relations. Solidworks' method of just suppressing the features or blocking actions that would fail features teaches them to either leave all the suppressed features for the next person or delete them and make new. Or even worse, instead of editing features to make the change(s) they just slap more and more features on the end of the tree.

I think you nailed it .. I seems that Dasult have gone to town of crafting UI components and forced upon workflow just to have end user to give up and slab everything that needs to be edit at the end of the feature tree.
In other words their own poor man "synchronic" workflow. One way modelling but they just haven't get the feature tree working to hide all the mess that its produces. Who knows .. maybe one day the button "Hide all mess" will be added to SW's cluttery UI.

Pernils wrote: ↑Tue Mar 12, 2024 10:16 am I think you nailed it .. I seems that Dasult have gone to town of crafting UI components and forced upon workflow just to have end user to give up and slab everything that needs to be edit at the end of the feature tree.
In other words their own poor man "synchronic" workflow. One way modelling but they just haven't get the feature tree working to hide all the mess that its produces. Who knows .. maybe one day the button "Hide all mess" will be added to SW's cluttery UI.

I fear suppressing down stream features was the solution to customer complaint, "Down stream features blow up when I edit my model!"

Pernils wrote: ↑Tue Mar 12, 2024 10:16 am I think you nailed it .. I seems that Dasult have gone to town of crafting UI components and forced upon workflow just to have end user to give up and slab everything that needs to be edit at the end of the feature tree.
In other words their own poor man "synchronic" workflow. One way modelling but they just haven't get the feature tree working to hide all the mess that its produces. Who knows .. maybe one day the button "Hide all mess" will be added to SW's cluttery UI.

I had a collegue that had "delete child features" unsupressed and he wouldn't pay much attention to anything. After a year of working by himself, he was wondering why he was having such long load times on his projects. When I looked at his master assembly, it had well over a thousand suppressed mates in that top level assembly alone.

That kinda left me wondering, what do people actually check when their files are slow? It also lead me to build a little training course inside the company to explain how to alleviate drawings, assemblies and parts.

CAD software is a "tool".
How much "training" did you get when you buy a hammer?
Was there instructions/warning not to hammer a screw or bolt?

Company need to establish a standard and train employees to that standard.
Most company just hand over the hammer and say "Go nuts".

Frederick_Law wrote: ↑Tue Mar 12, 2024 12:04 pm CAD software is a "tool".
How much "training" did you get when you buy a hammer?
Was there instructions/warning not to hammer a screw or bolt?

Company need to establish a standard and train employees to that standard.
Most company just hand over the hammer and say "Go nuts".

Shouldn't need to train people not to hammer screws or nuts.

bnemec wrote: ↑Tue Mar 12, 2024 12:35 pm Shouldn't need to train people not to hammer screws or nuts.

As I often tell my boss, common sense is not all that common these days.

bnemec wrote: ↑Tue Mar 12, 2024 12:35 pm Shouldn't need to train people not to hammer screws or nuts.

Doing that every day.

AlexLachance wrote: ↑Tue Mar 12, 2024 12:38 pm As I often tell my boss, common sense is not all that common these days.

Yeap, common sense went to another universe.
Call Dr. Strange to bring it back.

Pernils wrote: ↑Mon Mar 11, 2024 8:25 am
It sort of remember its reference. In other words it will gladly follow what end user want to do and not force its own stupid rule set on what is allowed.

Its amazing how broken this SW really is.

SE isn't showing a warning or error that I see, just the link icon if you edit the sketch, but its not obvious that its connected to anything. I guess its remembers the edge from history that isn't there anymore? Not really sure how I feel about that, like its linked to a ghost I can't see anymore.

The SW rebuild thing is an issue although minor in this case. Guess I've just gotten used to using on Force Rebuild instead of the faster regular rebuild. Unless you are doing extremely complex models with hundreds of features, force rebuild is a better option and about as quick. You can add the Force Rebuild icon to your toolbar.

jcapriotti wrote: ↑Tue Mar 12, 2024 3:48 pm SE isn't showing a warning or error that I see, just the link icon if you edit the sketch, but its not obvious that its connected to anything. I guess its remembers the edge from history that isn't there anymore? Not really sure how I feel about that, like its linked to a ghost I can't see anymore.
image.png

Going from memory, there are color settings that make it quite obvious what's broken. To know what it referenced; in the workflow I used, I would start under the feature I just suppressed and know that any new broken ref would be to the thing I just suppressed. Most of the time it was a small enough bite that there weren't that many possibilities. I should go back to SE to refresh my memory. I suppose it's one of those muscle memory things where I forget the details of how exactly it went until something quits working.

I think I'm finding new workflow(s) in SW to meet the same ends, just relearning muscle memory or new habbits.

Frederick_Law wrote: ↑Tue Mar 12, 2024 3:43 pm Doing that every day.

At the risk of being a jerk: https://www.dictionary.com/browse/capitulate

I get it, we don't have a choice much of the time. But it just seems if we keep on this path of replacing the expectation of reason with training, eventually we'll run out of people with enough logic ability to recognize the differences, on their own, between a nail and a screw. Hopefully I'm wrong.

bnemec wrote: ↑Tue Mar 12, 2024 6:22 pm At the risk of being a jerk: https://www.dictionary.com/browse/capitulate

Don't worry, we're all beyond that long time ago
We're here because we have strong opinions.

My point of view:
How long does it take to realize I'm hitting my head on the wall which won't go away.
And finally get up and walk around it.

SolidWalkAround