WTF is going on here ?

[Pernils]

I have a sheetmetal with some geometry.
The black is just to simulate some pieces from o-rings.

When I'm in the edit of the sketch of Boss-extrude2 ...

And press ctrl-q (as this seems to be the correct way to truly have your model up to date) ......

It sudden will crash most of the features .... What a hell ....

So the hidden rule is never ever use ctrl-q in sketch mode or what ?
And in what situation is this a must have behaviour ?

After 25+ year modelling I have never ever encounter a situation where I need a fast way to nuke my model.

[Glenn Schroeder]

Do not use Ctrl+Q when in an open sketch. I can't say why it messed up your features when you tried it without more information. If I was to speculate I'd say that maybe your edits of the sketch caused lost references, and they showed up as errors after Ctrl+Q since that workflow closes active sketches.

[AlexLachance]

I've never had trouble with CTRL+Q in a sketch, the only thing it does is it closes the sketch command to rebuild the entire feature tree, so if what you have in your sketch is problematic it will throw off errors, but in your case the feature is at the end and it throws errors on features before boss-extrude2, which is kinda weird.

Could you share the part...?

[Pernils]

Sure ...

https://drive.google.com/drive/folders/ ... sp=sharing

Nah.. this is a Eastern egg.
Its just me who have a hard time to find this useful.

[DanPihlaja]

What is going on with this cut?

[AlexLachance]

You don't need to edit anything, your Cut-Extrude1 loses it's reference upon a rebuild. Edit the cut and accept it and everything will be fine and dandy. Didn't re-happen after.


Most likely, features were moved around and SolidWorks fumbled in it's reference reassignement. Since it hadn't been "force-rebuilt", it wasn't showing the error until then.

[Pernils]

.. seem to be rock solid this designer tool ...

I don't know .. perhaps I'm becoming a SW user at all.
So this ...

.. that "Trough All - both" is just sudden is not a valid option in Hole wizard.

is just .. okay that's also broken ... so I have to work me around with mirror instead....

[RMcHugh]

I've been using swx since '96-'97 and have never known the hole wizard to offer through all-both.
I'm on '22 sp5 right now and it's not an option. Maybe it's in '23 or '24, haven't used them yet.

[AlexLachance]

.. seem to be rock solid this designer tool ...

I don't know .. perhaps I'm becoming a SW user at all.
So this ...

.. that "Trough All - both" is just sudden is not a valid option in Hole wizard.

image.png

is just .. okay that's also broken ... so I have to work me around with mirror instead....

I understand what you're saying but think of the hole wizard as a "tool" and not a feature. It is normal for it to not have through all both sides. If it was existing, then the occurences would need to sometimes exist, sometimes not, and the orientation would also need to sometimes be guided, sometimes not, which is why it is better to have it be left as it is and have the user mirror the feature or do it in a different manner.

I've been using swx since '96-'97 and have never known the hole wizard to offer through all-both.
I'm on '22 sp5 right now and it's not an option. Maybe it's in '23 or '24, haven't used them yet.

Honestly, I doubt it will ever be because of the complexity it brings forward. SolidWorks can't even determine which occurence is the seed occurence, let's not confuse it more.

[Pernils]

Honestly, I doubt it will ever be because of the complexity it brings forward. SolidWorks can't even determine which occurence is the seed occurence, let's not confuse it more.

Yes you are right there that SW is broken beyond repair and ask the dev to add/change or even repair will brake the tool even more.

I understand what you're saying but think of the hole wizard as a "tool" and not a feature. It is normal for it to not have through all both sides. If it was existing, then the occurences would need to sometimes exist, sometimes not, and the orientation would also need to sometimes be guided, sometimes not, which is why it is better to have it be left as it is and have the user mirror the feature or do it in a different manner.

But I think you are wrong here to not have the tool to not be consistent.


In the other CAD you are giving guidance's on where to cut with a regular cutout.

One side..

Both sides ...

The other side ..

In the "Hole Wizard"

We have the same on what side or both sides.
Hmm but we are missing the option for non symmetric on both sides. But on the other hand If we would have the option it surely would complicate callouts for the holes in the draft environment later on.

This is with regular or threaded hole but what will happen if I decide to use for example a countersunk hole.

Then the option for both sides is not a valid option.

One can argue that this is also is not a consistent behaviour but I find this to be more in the grey zone for that topic.

[AlexLachance]

Yes you are right there that SW is broken beyond repair and ask the dev to add/change or even repair will brake the tool even more.




But I think you are wrong here to not have the tool to not be consistent.


In the other CAD you are giving guidance's on where to cut with a regular cutout.

image.png

One side..

image.png

Both sides ...

image.png

The other side ..

In the "Hole Wizard"

image.png

We have the same on what side or both sides.
Hmm but we are missing the option for non symmetric on both sides. But on the other hand If we would have the option it surely would complicate callouts for the holes in the draft environment later on.

This is with regular or threaded hole but what will happen if I decide to use for example a countersunk hole.

image.png

image.png

Then the option for both sides is not a valid option.

One can argue that this is also is not a consistent behaviour but I find this to be more in the grey zone for that topic.

I'm not really sure what you're trying to get at? The fact still remains, the hole wizard is used as a "tool", not as a model generator. It then can be used to drive other things such as patterns. If the hole is as you say, then is it one fixation or two? Is it orientation A or is it orientation B?

BTW. I often talk very formally but I'm not a representative of SolidWorks, so I might be mistaken in what I say, but that is what I believe.

[SPerman]

so I have to work me around with mirror instead....

Be fore-warned. Solidworks definition of "mirror" only works in certain conditions. I can't fathom why the programmers think this is good.

I'm a GIF. Click me.

[AlexLachance]

Be fore-warned. Solidworks definition of "mirror" only works in certain conditions. I can't fathom why the programmers think this is good.

I'm a GIF. Click me.
mirror.gif

Hey Scott, try mirroring the body rather then the feature

[SPerman]

That was a quick example. Frequently you don't want to mirror the entire body, just a single feature.

[AlexLachance]

That was a quick example. Frequently you don't want to mirror the entire body, just a single feature.

True. For hole wizards, I try to recreate an entire feature rather then mirror it because there are too many times where we've started with symmetrical sides and ended up with non-symmetrical sides. I just attach the holes that need to be lined up together so if that one moves the other moves also.

[Glenn Schroeder]

Honestly, I doubt it will ever be because of the complexity it brings forward. SolidWorks can't even determine which occurence is the seed occurence, let's not confuse it more.

To be fair, they did address that problem a few years ago. It still happens to me occasionally, but much less than before they worked on it.

[AlexLachance]

To be fair, they did address that problem a few years ago. It still happens to me occasionally, but much less than before they worked on it.

"Still happens occasionally" is pretty much a resume of most of the issues they fix lol

I'm on 2023 SP4 and still get the seed issue fairly often. Consistently inconsistant I guess..?

[Pernils]

That was a quick example. Frequently you don't want to mirror the entire body, just a single feature.

Try to mirror constructions surfaces ...

It adds even more complexity with complex geometry that needs help of construction surfaces and projection if you also have to think ahead that you only can mirror the whole body.
There are complex geometry done in SW so its not impossible, but I think it needs way more hours to be good at then other CAD that have more robust help for the end user.

[acmall]

Be fore-warned. Solidworks definition of "mirror" only works in certain conditions. I can't fathom why the programmers think this is good.

Just in case anyone is reading this thread that doesn't realise what is happening with the mirror, it is trying to mirror the feature complete with the up to surface end condition so it ends up extruding back up to Plane 1 in the same direction. You can see this if you select full preview. If you select Geometry Pattern from the options it will mirror as expected as it only mirrors the geometry.

[SPerman]

Thanks for teaching me something. I wasn't aware of the "Geometry Pattern" option.

[Pernils]

Can confirm that it also mirrors geometry that have help of constructions surfaces.

Is there a situation where it will not produce a mirror if this option is not checked ?

[TTevolve]

I had this kind of thing happen with a tube that was extruded up to an assembly surface (in context) by a co-worker. I could not figure out why it was not growing or shrinking in length like other parts were in the assembly. It is great now that I know that is what it is doing.

When you do up to surface cuts/extrudes you need to be careful when doing patterns and mirrors.

[Pernils]

Here is something I don't quite understand why it best to have it like this.

We have some text on one side (A).
If I then change my mind to have the text on the other side with just using the option to change sketch plane.

Edit ...

Selecting the other side as sketch plane.

Then suddenly the text object is mirrored.
To me this seems to be a bit unwanted behaviour. Or are the some deeper thoughts behind this move by the devs ?

It even gets more weird when if you make a new protrusion and use the same plane and the result will not be mirrored.
I don't know .. is this some Easter egg trick to give the user the ability to have mirrored text faster instead of using the clumsy way by navigate throw the messy drop down menus ? ...

[josh]

Changing the sketch plane does NOT change the orientation of the sketch. It just changes the location of the sketch in space. Sketch text is just sketch entities. In order to read left-to-right on the opposite side of the part, the sketch would have to be rotated 180 degrees in addition to moving to the other side of the part.

[Pernils]

Changing the sketch plane does NOT change the orientation of the sketch. It just changes the location of the sketch in space. Sketch text is just sketch entities. In order to read left-to-right on the opposite side of the part, the sketch would have to be rotated 180 degrees in addition to moving to the other side of the part.

I assume this is not a regression during version bumping so they must have intentionally left this implementation in an broken state.

[josh]

I assume this is not a regression during version bumping so they must have intentionally left this implementation in an broken state.

*sigh* just because you don't understand it doesn't mean it's broken. Changing the sketch plane has never reversed the sketch normal. Because it shouldn't.

[CarrieIves]

@josh Is there a way to flip the sketch plane normal after a sketch exists?

[ryan-feeley]

@josh Is there a way to flip the sketch plane normal after a sketch exists?

Not josh, but yes there is. As you probably know, you can flip the normal of an existing plane, but that doesn't automatically propagate to any sketches that use that plane (which you can determine by viewing the plane's children). For the later:

1. Delete all external relations in the sketch. I expect you know how to filter the sketch relations to show these.
2. Do Tools > Sketch Tools > Modify.
3. A gizmo appears on the screen. RMB one of the dots to flip about the corresponding axis.
4. Re-establish any deleted relations.

Definitely CTRL+Q before and after doing this. But it does work. You may have some relations flip that you'll need to repair.

[josh]

You might be able to accomplish that by switching the plane through a couple of intermediate planes... But why? Just edit the sketch text and hit the button to flip it.

The 2 reasons why to somehow "rotate" or "flip" the whole sketch around (so the text doesn't look mirrored) would be wrong:

-Any sketch relations previously created to existing geometry would likely fail or screw up the sketch.
-How is SW supposed to know which way you'd want to "flip" the plane? Vertically or horizontally, that is. Is it supposed to try to analyze the geometry of the sketch and "decide" whether it ought to be flipped one way or the other?

[Glenn Schroeder]

@josh Is there a way to flip the sketch plane normal after a sketch exists?

One easy fix (notice I said easy, not pretty) that might work would be to do a circular pattern of the feature that created the text, then use a separate feature to remove the original.

[Pernils]

*sigh* just because you don't understand it doesn't mean it's broken. Changing the sketch plane has never reversed the sketch normal. Because it shouldn't.

I have 25+ year in a tool that sort of don't bother me to keep track of the sketch normal. From this experience I find SW's behaviour on the topic to be more in the way then actually helping the end user.

[Pernils]

Is there some cleaver thought behind why you only can select and not deselect (holding ctrl) parts in graphic environment ?

Its gets even more confusing if you select parts/asm from the part explorer and press mass property it sudden will exclude the mirrored parts/asm.

Here I have selected the items I want mass property on using the explorer.

After pressing mass property SW just keep excluding the mirrored asm.

But what happens if I select the parts/asm with box select ?

Then SW thinks its okay to keep the mirrored part.

We have also if you want to deselect items using the explorer (holding ctrl) you must click twice if you started your selections with box select in the graphical environment.

[josh]

You need to understand the difference between Features and Components.

[Pernils]

You need to understand the difference between Features and Components.
image.png

I haven't used so much asm features in the past but in this case its SW's lack of interacting with the end user.
What would happen for example if the mirrored asm have been hidden behind some other part ?

Just for comparison :

In SE 2022 if you select mirror feature in the path finder to check its mass properties.

You will get a warning that this is not possible

In later releases of SE it just works.