"Convert to feature" function ever coming?

[JST]

Solidworks has some capability for this, although I never had to use it, and am not entirely clear on how limited it is.

Basic issue:

My customer comes to me and has a model that he wants modified. The model exists ONLY as a STEP or similar model. It is not a simple part, and is something of a big nuisance to re-create. He does not want to pay for a total re-creation anyway.

I see I am not the only one, since there is another thread here on modifying an STL file part. And, there is is, the only option is to re-create the model, which several in that thread have said.

In Solidworks, at least some parts of a "dumb solid" model can be converted into "editable features". This is not currently possible with Alibre.

So, if a hole needs to be moved, or even changed, the procedure is to "weld it up", by putting IN a NEW feature that fills the hole, and then re-doing the hole wherever it is wanted. Similarly with bosses, edge chamfers/fillets, etc, all sorts of things that are actually simple and identifiable forms, and likewise are commonly changed.

If much more work needs to be done, it ends up being a case of recreating the whole thing as an Alibre file.

I do not claim that this is a primary function that has to be in Alibre for it to be a credible program. Obviously it is not an everyday use feature. HOWEVER, if this could be on the list, it would be a definite selling point to have it available. I do not compare features on high end CAD much, but as far as I know, only Solidworks has this.

There have been multiple cases in which I could have used it, but did not have it available. In each case, it took quite some time (unbillable in some cases) to work around the problem. I do have such a case in hand now, for instance. I did work for the customer previously, he insisted that all records be deleted due to patent disclosure issues, which I did, and now he wants modifications a couple years later. Naturally, he does not have the original AD model anymore.

 

[lamar]

JST
I would remodel the part. I use Solid works at work and their feature recognition is not that great. the software will not recognize the feature to how you would normally model the part, instead it will model it in some odd way and will not recognize all the features so you end up with a part that is not fully usable so you end up modeling the part anyway.

 

[DavidJ]

The Direct Editing Tools are specifically designed for working with imported parts - they allow change of hole/shaft diameter, move pocket or boss, deletion of faces (hence feature removal), etc. They would seem to do much of what you need.

 

[idslk]

Hello JST,

The Direct Editing Tools are specifically designed for working with imported parts

here a sample on an imported Step file:









It's worth a try...

Regards
Stefan

Edit:
Changing a hole:

 

[Lew_Merrick]

Hi JST -- See my response to Mareike in the "Modify STL model" discussion. -- Lew

 

[JST]

I actually do not like, nor often use, the direct editing. When I have, it seems clumsy and non-intuitive. I may simply not understand what to do with it.

It is easier to make another model than mess with it, so far. I have used it for VERY simple stuff.

I do not know how to move a hole with it, although I can make one deeper. However, I do not need the feature to do that, even with a dumb solid.

That may be because when I need it, I am in the position of learning to use it on-the-fly, which is not ideal.

 

[idslk]

I do not know how to move a hole with it

1) choose "Push Pull Pocket or Boss"



2) Select the input box "Selection" and than the faces you want to move



3) Select the input box "Direction" and than an axis or edge for the direction you want to move along



3) Select the input "Cone" and than the front point of it an move the selected faces (alternative you can enter a value in the box "Move Distance")





4) The value in "Move Distance" will also create an EquationEditor value.



5) the result is a feature in the explorer tree which can afterwards also be edited.



Regards
Stefan

 

[DavidJ]

Direct editing video

 

[HaroldL]

That may be because when I need it, I am in the position of learning to use it on-the-fly, which is not ideal.

Sounds like you need to set aside some time to learn about some of the other tools Alibre has instead of just relying on the standard ones. It's easy to get set/stuck/trapped in a particular method of modeling. After not using the Shapes I've started to use them for created radiused rectangular features and find they can save me a lot of time. Also Move Face and Remove Face have become real handy - once I became familiar with and learned how to use them.

 

[bigseb]

... Also Move Face and Remove Face have become real handy - once I became familiar with and learned how to use them.

+1

 

[JST]

OR, the standards committee could have not rolled over about an actually useful form of STEP file. That would be better, but it is a done deal now, and we know who the winners were..

Move face I have used relatively often.

For the other things, if more than just a few isolated items (and it usually is) then I would redo the model. Just not worth it when that is likely to be the end point anyhow.

"Pay me now, or pay me (more) later!"

Normally there are many things to be done to multiple faces of the dumb solid, with the face changed and moved as well, and you get into what comes first in order of operations. And then there are changes to that. And finally the case of "well *that* particular and essential change is not possible with the toolset". Phooey. Not so useful at that point. Good for "a tweak or two".

Nothing beats a real model with a feature tree.

Now, I expect to get flamed to a crisp for this (So I likely will not bother to check back here)..... BUT....

If Alibre wants to make some $$$, then a stand alone cut version of Alibre (at a cost, of course), aimed specifically at conversion of dumb solids would be interesting. That would presuppose "real" exports into more formats than now exist, however, so that no matter which of the big formats you use, you can use the converter..

The "convert to feature" COULD be made in a way that was more user-controlled and that would be useful, "choose base plane". "Choose extrude face" and etc. Would use the existing dumb solid directly as a guide to build the new model with the shapes being turned into real features in real time as you work, saveable as a standard model. It really comes down to the extraction of the base planes and sketch profiles. I do not think Solidworks did it right.

I see it as an extension of the existing tools, and NOT a totally new thing, but probably best as a separate "universal converter".

 

[HaroldL]

...The "convert to feature" COULD be made in a way that was more user-controlled and that would be useful, "choose base plane". "Choose extrude face" and etc. ...

That's an interesting proposition. How to implement is another matter though since any part you want to convert is going to be vastly different than any other part.

SolidWorks has a "convert" facility and the very few times I've used it the resulting part had more steps than if I would have recreated the part from scratch. Where a single fillet would have been used for several edges SW created multiple fillets; sometimes what could have been a revolve turned into several extrudes.

Each part you import that needs changes should be evaluated and either use the Direct Edit tools for minor changes or it's a complete rebuild.

 

[bigseb]

I'm familiar with this SW convert feature. Its ok. It misses design intent, I would rather model it in a way that could accommodate possible future design changes. So it not great but a cool idea. Honestly though I would much prefer a fix to current bugs and long-standing suggestions be implemented.

 

[JST]

........ Honestly though I would much prefer a fix to current bugs and long-standing suggestions be implemented.

For sure, that wins by a mile in my book. A person can ask, though.

That's an interesting proposition. How to implement is another matter though since any part you want to convert is going to be vastly different than any other part.

SolidWorks has a "convert" facility and the very few times I've used it the resulting part had more steps than if I would have recreated the part from scratch. Where a single fillet would have been used for several edges SW created multiple fillets; sometimes what could have been a revolve turned into several extrudes.

Each part you import that needs changes should be evaluated and either use the Direct Edit tools for minor changes or it's a complete rebuild.

I was thinking of a system where YOU do the thinking, and the MODEL supplies the geometry.

Essentially, the imported model is "there but not there". You get to pick planes on it to use, and you get to "project to sketch" from the imported model, but when you save the re-created model (which is what you would have), the original model is not part of it.

I would IN NO WAY want the program to do the thinking and converting. How would it know? That would need development.

Nuh-unh..... As I say, basically the imported model is used to fairly easily derive the sketches to re-create the model in Alibre. The imported model cold be shown as a variety of wire frame if desired.

The alternative way of re-creating the model is to laboriously measure, and create each sketch form measurements, BUT THE GEOMETRY IS RIGHT THERE IN THE ORIGINAL.

It makes sense to be able to DIRECTLY USE that geometry to create the skketches you need.

See, the issue with the move surface etc, is that inevitably, you either run up against something you CANNOT do in direct edit, or the thing gets to be a horrible overlay of original and changes that is essentially "tapped out" on your ability to use it further.

I wish I could show you the model I have and the changes.... Almost every surface has changes, ALL of which would be child's play if there was a native model.

As I continue to look at it, I just do not see any way of effectively doing it with tools available, and it will be a re-do. I have asked the client for the original drawing as well as the one showing the changes. Nada so far.

 

[DavidJ]

Here is a method that works, and potentially wouldn't need huge amounts of development to make it slicker (said the man who has no idea about how complex it really would be).

1. Import STEP (or other file) into Alibre. Save as Alibre Part.
2. Create new part, Boolean unite part from 1 above in this new part.
3. Create planes as desired, based upon the import geometry - Project to sketch from the existing geometry (don't use maintain association).
4. If you suppress the Boolean, you'll see your subsequent planes fail - so un-supress it.
5. Measure each plane created in 3 relative to the default reference geometry - edit each plane definition to work from the default reference geometry (and perhaps other planes from this set that you've already re-defined). If you are really organised, you'd define the plane this way to begin with and cut out a step.
6. You can now suppress the Boolean without causing failures - so you could now delete it. This leaves planes and sketches behind.
7. You'd need to add dimensions (or locks) to sketches to fully define them. Then extrude/revolve/etc.

You could use the same approach with planes to set 'extrude to' limits, making the 3D feature definition faster.

The slow bit in this is re-defining the new planes so that they are not dependent upon the imported geometry, I can see that becomes a pain if the geometry is complex. I can think of a couple of functional approaches (from user perspective) that could speed this up considerably ;-

1. Define planes in usual way, but have an option to also select a 'reference plane' that the new plane definition would be set relative to.
2. Have a 'Project Plane' this would be a 'one time' action - effectively the above option as a separate command, rather than integrated with the existing Plane creation tool.

Something similar would be needed for Axes and Points.


Maybe one of our Script experts can think about if the necessary functionality exists to provide some of this reference geometry creation / re-definition in a Script. I suspect simple cases may not be too difficult, but the more general case won't be easy to get right.

Just a thought - have fun trying it out.