Sketching Philosophy Question

[sgertsch]

Sketching Philosophy Question

I have just started to experiement with Alibre and feel that I misunderstand how to use the sketcher. From what can determine the resultant sketch always has to resolve to a "nice" chain of curves with no overlaps or bifurcation branches. It is not that I do not know how to trim the sketched curves to produce a vaild profile, but doing so invariably deletes import design constraints and I lose visually meaningful curves that help communicate design intent.

Does Alibre absoultely require sketches to be "nice" to be usable in a 3D modeling operation?

Note: Prior CAD experience is with I-DEAS where sketch curves are used to facilitate creation of "sections" (profiles), which are in turn used for modeling operations.

I also find it difficult to detemine a sketch's constraint schema visually. Outside of simple dimesional constraints I cannot visually see any information related to parallism, symetry, etc. What is the best practice to validate the behavior of a sketch?

 

[bobster]

In my experience with IDEAS, Pro-Engineer and Unigraphics all of these modlers sketchers are very similar to the sketcher in Alibre, but Alibre's sketcher is a bit friendlier and easier to use.

Constraints are visible, it does take a little close looking to see each constraint symbol. All constraints are available explicitly under the constraints button in the sketcher toolbar. The help screens and the manual do a good job of explaining each of these constraints and what the visual ques look like. This constraint display can be toggled on and off via CNTRL+SHIFT+C keyoard command or under constraints in the view menu. The size of the displayed contraint symbol can be increased via the tools, options menu.

All sketches need to be closed before they may be extruded, swept or revolved but the sketch does not need to be fully constrained, although it's good practice to fully constrain sketch geometries. Closed sketches are required in all modelers if I remember correctly.

There is an analyze function available under the sketch pull-down that is very useful and provides a visual display as well as text description.

Alibre allows you to auto dimension a sketch, this is also useful when a DOF remains and you can't figure out where it's hiding.

 

[lens_cad]

In the sketcher, any sketched figures can be converted to reference figures. Reference figures appear in the sketch and can be used to constrain regular figures, but they are not used to create solid geometry directly.

Len

 

[jwknecht]

Re:

In the sketcher, any sketched figures can be converted to reference figures. Reference figures appear in the sketch and can be used to constrain regular figures, but they are not used to create solid geometry directly.

Len

That is what I was going to suggest too.

Coming from IDEAS too. Had the same issues for awhile. Chalk it up to getting used to a little different interface. Now, I am used to Alibre's interface.

What I think is bothering you coming from IDEAS (because it bothered me at first too): In IDEAS you create all your sketch geometry not worrying about trimming corners off corners, etc. After your sketch was made, you are then required in IDEAS to select which of the sketch geometry will be your sketch profile. In Alibre, all sketch geometry that is not turned into reference will be by default your profile.

One thing I did like about IDEAS is that it showed by color code how constrained each sketch figure is. In Alibre, you look at your DOF for the sketch at the bottom of the screen and also you can (with a constrain tool selected) mouse over the sketch figures and it will say underdefined, well defined.... Also, IDEAS has the option to animate the sketch to show how it is not constrained, which is useful. What I do in Alibre when I run across a sketch that is not fully constrained (DOF), I will autoconstrain to see what pops in.


All in all, just a matter of getting used to it. Stick with it and I am sure you will end up liking it.

EDIT: By the way, I am kind of weird and actually read the Alibre User Guide cover to cover before I purchased the software. It helped and actually did not take very long.

 

[Gaspar]

Re:

...Constraints are visible, it does take a little close looking to see each constraint symbol...

From the options menu you can select "large" constraint symbols.

...All sketches need to be closed before they may be extruded, swept or revolved...

If needed, open sketches can be extruded (swept or revolved) with the "thin wall boss or cut" available in the feature menu.

In my experience with IDEAS, Pro-Engineer and Unigraphics all of these modlers sketchers are very similar to the sketcher in Alibre, but Alibre's sketcher is a bit friendlier and easier to use...

Thanks for sharing. I've only used Alibre and it's reasuring to listen that we are standing on firm terrain from someone with your background :wink:

 

[moyesboy]

while the sktch can be extruded as thin wall when it is an open loop (eg U, L, N, M, C) it cannot be extruded with a any biforkation (e.g. Y, E, K, A, P) which is a pity...
:cry:
I still hope for a way to put a cross section on a 3D sketch of any complexity, loops, forks etc - in one operation.

 

[Gaspar]

Moyesboy,

I had never tried it, but I seemed to be able to extrude thin wall bosses with bifurcations... (I just emailed you the original file)

 

[bobster]

Gaspar,
You're right, I never tried to extrude an open sketch, but I tried it, it does indeed work, I just learned something!

 

[Gaspar]

 

[jwknecht]

Re:

Moyesboy,

I had never tried it, but I seemed to be able to extrude thin wall bosses with bifurcations... (I just emailed you the original file)

Gaspar, I use extrude for thin wall all the time, but I have never seen anything like that. What am I seeing? Is Moyes curved (the text, not the man)? Can you post your file in the Binaries?

 

[Gaspar]

Done...

 

[sgertsch]

I want to thank everyone for their comments, especially the pointer about using reference figures. Sketching reference figures first and then follow-up with plain old figures addressed my concerns (problem). I didn't initially consider using reference figures because I associated them with something in I-DEAS called "Reference Curves", which are used to make sketch curves visually persistent, and therefore reusable, at the part (solid model) level.

The suggestion to turn on "Large constraint symbols" option helped, but there are still a lot of constraint conditions that I know exist but are not graphically shown. For example, if I used the equivalent "rectangle" sketching tool in I-DEAS the result would clearly show the parallel and perpendicular constraints that maintain the design intent (rectangular shape).

Another thing I am a little uneasy about (as I learn to use Alibre) is having confidence in the sketch behavior relative to dimensional change. In the I-DEAS "sketcher" (during constraining) color-coding is used communicate the Degree Of Freedom (DOF) state of individual curves. There is an "Show Free" function which can be used to graphically preview-animate what will happen to unconstrained, or partially constrained sketch geometry. But most importantly, there is a "Drag" function, which allows the user to increase, or decrease a dimensional nominal value (by simple mouse movement) and see, in real-time, the effect on the sketch.

The ability to clearly see and validate design intent is a critical component in any CAD tool that supports an iterative design process; in the sketching area Alibre this appears to be deficient. There are many capable 3D modeling tools out there, but there is a significance difference between using a CAD product for 3D rendering and one that truly supports an iterative design process.

 

[ideazonepd]

It is true that the 2D sketcher in Alibre does not visually (read: color-coded) show the remaining Degrees of Freedom and the figures they correspond to. But it does show the number of DOF remaining as a number in the lower right corner. The Auto Dimension tool is also very useful. Sometimes I find that I can't figure out what the remaining DOF would be. So I use the Auto Dimension on all figures and it shows what is still free to move. Sometimes I don't like the way it inserted the dimension, so I'll hit Undo and do it myself. But it helps to know where to look.

One tip I would offer is to never leave a sketch without making sure that the DOF readout shows 0.

Good luck.

Myles

 

[demarchi]

Hi,
I used to work with I-Deas too. The sketch approach in I-Deas is rather unique, as the work bench / Bin. Alibre is more similar to many other 3D Modeler, and coming from I-Deas it takes some time to get used to the new way.
Consider there is also the "project" option, where you can decide if the profile will be associative and if it will be a reference line. This is equivalent to the reference curve in I-Deas.

Massimo

 

[HaroldL]

Sketching Philosophy Question

Another trick you can try, in addition to checking the DOF, is to click on an end point of a line in your sketch then drag it to see what moves. You can then apply dimensions or contraints to lock down the sketch.

BTW, my experience is with I-DEAS also. There seems to be a few here that have that in common.

HaroldL