CAD Forum

One thing I really miss about NX is the ability to edit sketch dimension values without editing the sketch. Is NX the only software with this functionality?

NX has a "dependencies" window, that lists the relevant values for a feature. So if you click on the sketch in the history tree, all of the sketch dimensions are listed. You change the value of a dimension, and everything else updates. (Depending on how your software is setup.)

The quality of my example is poor. I haven't used NX in a long time, and didn't waste time prettying things up for this example.
I'm a GIF, click me!

They must've added that after the version I last used (NX4). The closest thing I can think of in SolidWorks is either double click the feature and edit the dimensions on screen. Or open the equation manager, select the "Dimension View" and edit the dimensions.....however that list is not filtered and can get quite busy unless you rename your features to filter on.

You can sort of do this with Solidworks.

But you have to have Instant 3D on.


Once you have instant 3D on, you can double click on a feature and all of it's relevant dimensions show up....then you can click each one and modify at will and everything is updated immediately.

Solidworks has done a great job of adding efficiency to the software. Mouse gestures, bread crumbs, etc. all eliminate mouse clicks and make the user faster. But they've missed the fact that the overall layout could improve efficiency. Having the assembly navigator separate from the part navigator makes it much easier to find the feature you are looking for without all of the collapsing, expanding and scrolling. Some of this seems so obvious I'm surprised other companies haven't copied the functionality.

@SPerman are you switching to NX?

Solid Edge has something similar in assemblies: Peer Variables. It is an amazing tool for assembly work.

Mostly I'm just reminiscing, but there was always a chance that SW had similar functionality I was unaware of. I really want to switch to NX, but I can't justify the added cost.

Solid Edge has the Variable Table. Some models I would use it a lot, others not so much; depends on what the part was doing. It just shows every variable in the model, your screen shots look like there's a tree view of dependency? I don't know of anything like that in SE.

In Solid Edge this window can stay open while working in the model. Edit sketches, add features etc. Then tweak them from the Variable Table window and watch the model update; any dimension or feature property can be edited, patterns included. I have not figured out how to do the same in Solidworks.

Thanks. I will have to look at that in SE. In NX, it only lists the variables for the sketch/feature you have selected, so you don't have to filter the entire list. I think you can do the same thing in NX be selecting the top level assembly.

SPerman wrote: ↑Tue Sep 20, 2022 5:43 pm Thanks. I will have to look at that in SE. In NX, it only lists the variables for the sketch/feature you have selected, so you don't have to filter the entire list. I think you can do the same thing in NX be selecting the top level assembly.

I can see the active filter being nice an a big model, I don't recall trying this in SE. This is where I would name all my dimensions that I cared about or had functionality/design intent. So that would group them due to the sorting by name, kinda like "favorites" in a way. All the equations/formula was done here as well, so if I wanted something to be 2x thickness or whatever I'd do it from the Variable Editor usually.

jcapriotti wrote: ↑Tue Sep 20, 2022 2:39 pm They must've added that after the version I last used (NX4). The closest thing I can think of in SolidWorks is either double click the feature and edit the dimensions on screen. Or open the equation manager, select the "Dimension View" and edit the dimensions.....however that list is not filtered and can get quite busy unless you rename your features to filter on.

image.png

You CAN sort that list by clicking on the bars at the top. So can at least get it alphabetically.

AND you can also filter it (I see now that you did mention this.....oops....I will leave this here though):

Solid Edge has Dynamic Edit that can be invoked when an Ordered feature is selected that shows the features dimensions/sketch. Dim values can be edited and sketch elements dragged if underconstrained.

In Sync mode, dimensions appear when the face/s they control are selected and of course faces can be dragged too.

Both of these work at the part level or assy level where the part is placed.

Hard to say. I am used to the NX method but the SW paradigm of having all feature info visible and available for double-clicking in the tree, irrespective of what level of the assembly is currently active, also has its advantages. Often kinda wish that NX had this also.

For me, what makes NX way more powerful in the sketch-edit arena is the ability to choose sketch edit WITHOUT rollback. It can be a bit confusing at first, because you can't do the "temporal paradox" and select geometry that is actually downstream, but it is often really helpful to be able to do the sketch edit in the display context of what happens later.

Inventor, make sketch visible and you can double click on any dimension to change it.
Once it's visible, you double click dimension in another sketch to edit and select dimension in any visible sketch to use them in equation.

Hi Guys,

Solid Edge provides some solutions to edit a model without model history rollback (editing the sketch):

On part level:
Variables
Dynamic Editing

On assy level:
Peer variables
Face priority with Dynamic Editing

Here is a short video to this:


BR,

both of those last posts talk about editing sketch dimensions without rollback, which you can do in SW as well.

what I didn't see in the SE video (though I may have missed it): NX allows you to fully open a sketch and change all its content without model rollback. You see the model at its (later) state but you can go ahead and change everything in the sketch, not just the dimension values. You can add, delete and modify geometry freely. The changes don't get propagated until you call a rebuild.

It's sometimes hard to understand how useful this is, if you haven't ever worked this way before. Since you can still see all the geometry from features downstream from your sketch, it makes it much clearer as to what your changes will actually end up doing. As said in my previous post, what you can't do is create relations/dimensions to this downstream geometry. NX just won't recognize it for clicking, which can be confusing... would be nice if there was some kind of "can't pick this" symbol or such.

Jim Elias wrote: ↑Wed Oct 05, 2022 3:04 pm NX allows you to fully open a sketch and change all its content without model rollback

Did that in IV.
I think I did that in SW.

Jim Elias wrote: ↑Wed Oct 05, 2022 3:04 pm Since you can still see all the geometry from features downstream from your sketch

Master Sketch and SSP

Frederick_Law wrote: ↑Wed Oct 05, 2022 4:38 pm Did that in IV.
I think I did that in SW.


Master Sketch and SSP

Last IV job I did was 2016. I don't recall IV working the same way, but there might be the option. SW always rolls back on activating sketch edit.

I tried that master sketch / ssp stuff and never warmed to it, it always seemed to me like I was dealing with a stack of workarounds on workarounds. Plus the fact that geometry changes to the master sketch could often cause all downstream models to disintegrate. Guess it all depends on what you're designing.

Change in SW will blow everything up.
It doesn't maintain entity ID.
What it feels like is a creation list.
If you add entity, it go to end of list everything is fine.
If you delete ab entity, everything after that got move up and blow up.
Another funny is, SW will recreate the list sometime when you change something. Again all blow up.

IV is more stable.
And yes, modify sketch in IV will hide everything after it.
You can show the sketch and change dimensions without editing the sketch.

Frederick_Law wrote: ↑Thu Oct 06, 2022 8:33 am
(snip)
And yes, modify sketch in IV will hide everything after it.
You can show the sketch and change dimensions without editing the sketch.

thought so, that's a pity that IV also works that way.

off-topic: now what I really like about IV is how painless it is to re-attach dangling drawing dimensions. NX has an arguably more powerful system around drawing dimension geometry referencing, but re-attachment is more time-consuming than in IV for only a bit more flexibility. SW has unfortunately remained prehistoric by comparison regarding this.

Jim Elias wrote: ↑Thu Oct 06, 2022 10:09 am thought so, that's a pity that IV also works that way.

off-topic: now what I really like about IV is how painless it is to re-attach dangling drawing dimensions. NX has an arguably more powerful system around drawing dimension geometry referencing, but re-attachment is more time-consuming than in IV for only a bit more flexibility. SW has unfortunately remained prehistoric by comparison regarding this.

Sounds like Solid Edge and Inventor are closer in these behaviors. Drawings in SW feel like a big step backwards for us coming from SE.

Concerning seeing the built model while editing an earlier sketch, unless the software does an excellent job of automatic selection filters so that downstream geometry/bodies/surfaces/sketches are not selectable I can see that being a disaster. I have not had opportunity to use NX but from what I've heard it probably implemented this in a way to prevent the bumbling user from creating relations from the sketch to downstream geometry. I still struggle with this concept in an ordered environment though; maybe if I've used it I would love it.

bnemec wrote: ↑Thu Oct 06, 2022 11:59 am Sounds like Solid Edge and Inventor are closer in these behaviors. Drawings in SW feel like a big step backwards for us coming from SE.

Concerning seeing the built model while editing an earlier sketch, unless the software does an excellent job of automatic selection filters so that downstream geometry/bodies/surfaces/sketches are not selectable I can see that being a disaster. I have not had opportunity to use NX but from what I've heard it probably implemented this in a way to prevent the bumbling user from creating relations from the sketch to downstream geometry. I still struggle with this concept in an ordered environment though; maybe if I've used it I would love it.

You can't pick the downstream geometry, it won't highlight when you pass the cursor over it, etc. When I started with NX, I would sometimes go nuts trying to figure out why some things just weren't pickable, until I would realize -- that's the Ghost of Geometry Yet-to-Come, d'oh. (Probably a natural learning stage coming from systems that force rollback.)

Like I said in an earlier post, I wish the implementation was more elegant, maybe like showing downstream geometry in some other line font or color. But it doesn't take much to get used to as is.

NX calls the direct editing tools "synchronous modeling", but I think that this is just a marketing confluence to SE. Each "synchronous" operation adds a feature to a good old history tree, so it really is an "ordered" environment. There was a "history-free" mode a while back that was kinda like the SE synchronous environment, but it got killed off around NX10, apparently it wasn't well-received. I've seen rumors on the Siemens forums that it might come back though.

Jim Elias wrote: ↑Thu Oct 06, 2022 1:29 pm You can't pick the downstream geometry, it won't highlight when you pass the cursor over it, etc. When I started with NX, I would sometimes go nuts trying to figure out why some things just weren't pickable, until I would realize -- that's the Ghost of Geometry Yet-to-Come, d'oh. (Probably a natural learning stage coming from systems that force rollback.)

Like I said in an earlier post, I wish the implementation was more elegant, maybe like showing downstream geometry in some other line font or color. But it doesn't take much to get used to as is.

NX calls the direct editing tools "synchronous modeling", but I think that this is just a marketing confluence to SE. Each "synchronous" operation adds a feature to a good old history tree, so it really is an "ordered" environment. There was a "history-free" mode a while back that was kinda like the SE synchronous environment, but it got killed off around NX10, apparently it wasn't well-received. I've seen rumors on the Siemens forums that it might come back though.

That does sound nice. Most of what I've heard about NX is that most of the features/behavior is polished to a nice finish vs "If it kinda functions ship it." mentality.

The only time I remember crashing NX was in the Nastran simulation. The modelling side was VERY robust (circa 2016). That's not to say it didn't have its glitches, but it makes a SW SP5 release look like a beta project. Maybe if you want that kind of stability you have to pay NX kind of pricing.

Am I correct in remembering that you can reference dimensions downstream? Not geometry, but the sketches that drive the geometry?

bnemec wrote: ↑Thu Oct 06, 2022 1:48 pm That does sound nice. Most of what I've heard about NX is that most of the features/behavior is polished to a nice finish vs "If it kinda functions ship it." mentality.

SPerman wrote: ↑Thu Oct 06, 2022 2:01 pm The only time I remember crashing NX was in the Nastran simulation. The modelling side was VERY robust (circa 2016). That's not to say it didn't have its glitches, but it makes a SW SP5 release look like a beta project. Maybe if you want that kind of stability you have to pay NX kind of pricing.

yes, I've often thought that the high price of NX is driven by the consistent high quality level of the software engineering. It's not always perfect but it's definitely more dependable than what the others are doing.

Am I correct in remembering that you can reference dimensions downstream? Not geometry, but the sketches that drive the geometry?

Every driving dimension is given a parameter name that can be directly typed in at any prompt which would require compatible input (much more convenient than needing to go into a list every time). One peculiarity in NX is that you cannot re-use the values of driven dimensions (as opposed to e.g. SW, where you can use driven dimensions in equations). In NX, you need to do a separate "measure" feature, from which the output then can be used further.

DanPihlaja wrote: ↑Tue Sep 20, 2022 2:45 pm You can sort of do this with Solidworks.

But you have to have Instant 3D on.


Once you have instant 3D on, you can double click on a feature and all of it's relevant dimensions show up....then you can click each one and modify at will and everything is updated immediately.

image.png

That should work without having Instant 3D on. Just double-click a sketch or feature in the tree and dimensions should appear on screen. You can double-click and edit the dimensions in the dialog box. If you click the green checkmark you exit without immediate updating of the dim. Edit more dim's if you want to, either in the same sketch/feature or a different one. If you click the stoplight, the dimension and any others you've changed will update, but you don't exit the dialog box you're in until you click the green checkmark. I find it safer to rebuild with each dimension change.

Erik wrote: ↑Sun Nov 06, 2022 5:03 am That should work without having Instant 3D on. Just double-click a sketch or feature in the tree and dimensions should appear on screen. You can double-click and edit the dimensions in the dialog box. If you click the green checkmark you exit without immediate updating of the dim. Edit more dim's if you want to, either in the same sketch/feature or a different one. If you click the stoplight, the dimension and any others you've changed will update, but you don't exit the dialog box you're in until you click the green checkmark. I find it safer to rebuild with each dimension change.

Yes, but with instant3D on there is instant change as you change the dimension. With instant3D off, you have to hit the stoplight or CTRL Q to see the updates.

Erik wrote: ↑Sun Nov 06, 2022 5:03 am . . . I find it safer to rebuild with each dimension change.

Do you mind if I ask why you prefer manual rebuilding? I'm curious, not arguing.

SPerman wrote: ↑Thu Oct 06, 2022 2:01 pm Am I correct in remembering that you can reference dimensions downstream? Not geometry, but the sketches that drive the geometry?

Same with IV. You can use dimension (parameter) from last feature in first feature and anywhere in between.

Glenn Schroeder wrote: ↑Mon Nov 07, 2022 8:43 am Do you mind if I ask why you prefer manual rebuilding? I'm curious, not arguing.

Most of the time rebuilding to check that the change doesn't cause any unexpected changes before exiting the dialog box takes practically no time and only costs you one click. If something unexpected happens you can catch it right away. Making many changes and then rebuilding makes it harder to figure out what went wrong if a mix-up or typo you made (we all do it) somewhere in the course of changing all those dimensions causes an error.
On a big complicated model that takes ages to rebuild, it makes more sense to get many dimensions changed at once and then rebuild in one go. On the other hand sometimes those are the models best modified one step at a time.