Poor handling of failed features

[moyesboy]

Poor handling of failed features

When you edit something at the beginning of the feature history you will often find some features later in the feature history fail. This is becuase they depend on some geometry that can no longer be found - such as a sketch was on a face that was created with a line that was deleted from a sketch.

To prevent this you must be careful how you edit sketches and try to keep all the relevant sketch features present in the sketch when you edit it. Not always possible.

Inevitably you will sometimes end up with failed features.
Unfotunately I'm finding quite often that these features are diffcult or impossible to fix. Sometimes it is possible to change the defining sketch - however it is not possible to define a new plane for an existing sketch. Thus when you make a feature depend on a new sketch you first had to draw the sketch again then, because all the geometry it creates came from new lines a few more following features fail
If you have to delete the feature and insert a new one then of course now all the dependent features go into intalics
I think the other packages I have used handle this a lot better than alibre.

Here's what support said to me:
"COMMENTS:
Unfortunately you cannot delete the reference geometry/feature for another feature. Doing so will cause the feature to fail. In some specific instances you can replace the reference sketch, but not in all cases. The best way around this is to keep this in mind while designing. Make your design modifications first, before placing holes or other similar features".

Well I'm sorry but if I knew how my design was going to be and what features it would contain from the start the job would be a whole lot easier for all of us. In fact I wouldn't need a parametric design system at all because I wouldn't need to go back and make changes to the part as I developed the part design. I'd just create it right first time!

It seems you can just leave the failed features there and the 3D geoemtry is still created. So are many alibre users just leaving their parts with italicised (failed) features in them - saving up problems for later?

 

[warburton1]

In general terms I try to repair them when I discover them, primarily to prevent additional problems cropping up later in the design process.

One thing I find useful is to construct a skeleton part in geometry first. Usually this takes the form of limiting planes, lines and points. These items are easy enough modify and there use helps prevent the geometry changes causing the failures (target not available error?). However, the support for wireframe in Alibre leaves a little to be desired.

Skeleton modelling is perhaps the best technique for helping to prevent this type of error from occuring in the first place. On the other hand, I agree wiuth you, Alibre should have an "ability" to repair errors e.g. swapping sketch planes, isolating geometry that has lost its parent etc.

 

[fitzbond]

I've requested a redefine command that would allow users to redefine references for sketches and planes etc. the same way users can redefine constraints in assemblies.

 

[moyesboy]

One thing I find useful is to construct a skeleton part in geometry first. Usually this takes the form of limiting planes, lines and points.

But this is like making a 3D sketch if the design first before you creatre it in 3D solid.
It is better if the system that creates the 3D design is actually used for the initial desing too.
The lack of tools for sketching on different workplanes before crating 3D solid would make this layout method quite difficult - I totally agree there.

Alibre has good functionality for the price, but if you have used another 3D solid system then you find these holes in the functionality quite annoying. The workrounds are very time consuming. The reworks because you cannot redifine and fix things are also very time consuming.

 

[moyesboy]

I'd just like to add that failed features and having to recreate features has a severe knock on to 2D detailing in that when features cannot be repaired then dims become detached and need recreating.
Ususally the dinesnion go onto the dissociated layer which by default is red.
However on one occasion so far I had the dimensions just vanish which is not acceptable because you end up then applying the dimensions slightly differently when a part is revised (eg from a different edge), or maybe miss one off that was previously there.
In this case on opening the drawing I could see the dimensioned view, then came the parts has changed warning asking to update. After update the dimesions just vanished rather than turning red. I closed and opened the drawing again to check and the same thing happened again.
I had to complete the work and didn't retain the old files to send to Alibre support unfortunately.

 

[flyboydave]

Re:

I've requested a redefine command that would allow users to redefine references for sketches and planes etc. the same way users can redefine constraints in assemblies.

Oddly, you CAN redefine sketch plane references in holes, just not in sketch-based features. But like everything else that doesn't work quite right, it requires a workaround. You can't just pick the face you want. You have to select the face from the faces list in the design explorer. So the capability is there, its just not wired up, as there is no way to access a selection box for a sketch.

 

[flyboydave]

Re:

Alibre has good functionality for the price, but if you have used another 3D solid system then you find these holes in the functionality quite annoying. The workrounds are very time consuming. The reworks because you cannot redifine and fix things are also very time consuming.

Annoying, and costly. It's the difference between price and cost. Yes, it is low price, but all the workarounds cause a great cost. Anyone have an answer as to why any time you change a sketch, part, or assembly constraint dimension value it takes about 30 seconds to update? And this is on a smokin' dual-core 3.6 Ghz Dell PC with 2 GB of ram.

As a side note, I found a funny one - open an assembly with sheet metal parts. Shift-Edit one of the parts. Flatten the part. Go back to your assembly - the part is flattened in the assembly too. If you have lots of things constrained to that part, they will all be either failed, or will have flown out into space depending on their constraints. I haven't tried it, but I bet if you save a part in flattened mode and later open the assembly the same thing will happen.

Sometimes you can rebend the part and everything will fix themselves in the assembly, sometimes you just have to close it all (and lose any changes since your last save) and start over.

 

[flyboydave]

Re: Poor handling of failed features

When you edit something at the beginning of the feature history you will often find some features later in the feature history fail. This is becuase they depend on some geometry that can no longer be found - such as a sketch was on a face that was created with a line that was deleted from a sketch.

snip

It seems you can just leave the failed features there and the 3D geoemtry is still created. So are many alibre users just leaving their parts with italicised (failed) features in them - saving up problems for later?

First, italicized features and failed features are not the same thing. They are caused by similar actions, but they are different. A failed feature gets a red "x" through it, as well as any later features dependent on that one. A failed feature will not generate geometry.

An italicized feature will show "target no longer available" if you check its status. Those can be fixed. Usually, you can just edit its sketch and delete reference geometry that is hanging out in space, or does not have any dimensions attached to it. Keep that in mind when you read the message from support, as I think they were referring to failed features, and you were thinking about target no longer available (italicized) features.

I always fix all italicized features, as leaving them in can cause screwy behavior when you make changes down the road. And yes, other packages handle this situation a lot better. Some make you fix the problem right then to prevent later problems, and they all tell you exactly which references are lost so when you edit the sketch with the broken references, they are in a different color so it is obvious which ones need to be fixed.

But some of the italicized features can be reduced with different modeling techniques. For example, I've been working on these sheet metal enclosures with lots of baffles and panels in them, but you can do it with any assembly. Anyways, they all are screwed to a main chassis part. The chassis is the first part, but I don't put any mounting holes into it. As I create the baffles, I put holes into the mounting flanges at nice pretty distances, like 1/2" in from each end, centered in the flange. I build everything in top-down mode but minimize sketch constraints that reference other parts. I locate the parts with assembly constraints. Then once everything is in position, I add holes in the chassis using centers of holes in the flanges as their locators, no dimensions.

Then if you need to edit either the hole locations within the flanges, or the location of the flange itself, you just change it in the flange itself, or its assembly constraint. The holes in the chassis will move automatically.

Think of how many changes you'd have to make with all holes individually dimensioned within their respective parts - you'd start with broken constraints, and have to change hole dimensions in multiple parts.