Quick and Accurate SketchingOthers Friday, March 26th, 2010
Just about everything in parametric solid modeling starts out with a sketch and then involves more and more sketches as the modeling progresses. Sketching ends up taking up a significant amount of modeling time and CAD vendors have been trying to make it easier and faster for users to create and edit sketches. Normally sketching works like this. You already have a picture of what the sketch looks like in your head. Keeping that as a reference you click around the sketch plane creating lines, arcs, circles, etc. Once you are done your sketch looks pretty much like how you imagined it. You then go ahead and dimension the curves and add constraints so that they accurately represent the feature that you want to model.
In Inventor 2011 Autodesk has tried to merge these two processes (drawing and dimensioning/constraining) into a single efficient process. Now you can specify lengths and angles as you are drawing. Inventor automatically converts the lengths to linear dimensions and angles to angular dimensions. Take a look at this video.
Notice that in order to fully define the sketch I needed to add a dimension to only one line segment. Sometimes you do not need to do even that. All the other dimensions and constraints were applied automatically by Inventor as I was sketching. This is a huge time saver and a great productivity enhancement.
Now this feature already existed in AutoCAD and Autodesk claims that they simply took it from there and put it into Inventor. True. But not many may know that another company beat them to it. Take a look at this video.
This is the same sketch created in Alibre Design V12 which was released a few months ago. One of the key enhancements of V12 was this AutoCAD style sketching. As you can see the sketching in Inventor 2011 works exactly the same as it does in Alibre Design V12.
And since I am in the mood of comparing lets see what SolidWorks 2010 has in store for us. There is an option in SolidWorks called “Enable on screen numeric input on entity creation“. You can find it in System Options > Sketch. Turning it on will let you enter lengths as you sketch in the graphics window. No angles, just lengths. Take a look at this video.
Note that while you end up accurately creating curves, SolidWorks does not automatically dimension them and apply constraints. You still need to go ahead and apply them manually, which makes the whole exercise rather pointless. I guess that is why SolidWorks has turned that option off by default.
Reader Dan Lanigan pointed out that SolidWorks does have an option to automatically add dimensions as you enter values in the length edit box in the graphics windows as you sketch. When you are in Sketch mode check the “Add Dimensions” box in the “Options” tab in the panel on the LHS. However, unlike Alibre Design and Inventor, you can enter only lengths and not angles.
Let’s take a look at Solid Edge ST2. I couldn’t find an option to turn on like I did in SolidWorks 2010. But as you sketch you can enter lengths and angles in the edit boxes on the left pane. The pauses you see in the next video are due to me entering lengths and angles in the edit boxes.
I found this pretty irritating because I had to constantly change my focus between the graphics window and the left pane a number of times, which was not the case with Inventor, Alibre Design and SolidWorks. Also the Smart Dimension feature in Solid Eedge ST2 is not that smart after all. Clicking two non-collinear contiguous line segments wasn’t enough to let it know that I wanted to add an angular dimension.
Reader Jon Sutcliffe pointed out that Solid Edge has an option called IntelliSketch in the Sketching tab that allows automatic creation of dimensions as you sketch in the graphics window. However, unlike Alibre Design and Inventor, the lengths and angles cannot be entered in the graphics window where the mouse and hence user’s focus is. Rather they appear on the panel on the LHS which, as I mentioned above, is quite irritating because you need to continuously switch your focus between the graphics window and the left panel.
What about Pro/ENGINEER? It does not have this feature either. Or at least I could not find a way to turn it on because Pro/ENGINEER’s options box is a joke – an antiquated one. There are a zillion option variables with names like copy_geom_update_pre_2000i_dep and I didn’t have the patience to figure it out for myself.
The reason I brought this up is related to something Al Dean said in yesterday’s interview:
My point is that there are a huge range of tools out there that never get seen, never get looked at in any ‘depth’. Now. Why is that? Is it because the ‘CAD Press’ only ever attend events that they’re invited to, that they’re comped for? A little bit, yes. Is it because there’s a steady stream of information that’s sent out that can be used? Yes. Do they bother to go out and find new tools, new developers that just want to get their product out there or conversely, talk to older vendors that haven’t seen much action in years but have a compelling solution? No. I don’t believe they do for the most part.
Smaller CAD systems like Alibre Design continuously come up with some really nice enhancements and features. But I don’t think they get the attention they deserve. I try and look at CAD systems other than the mainstream ones. That has resulted in my blog series on PowerSHAPE 2010 and KOMPAS-3D V10. I am a programmer first and a user later. So my exposure to these CAD systems is rather limited. That’s why I have opened up this blog to readers so that they may contribute to it and share their experiences with the CAD systems that they use. If you feel like doing so, please click “Contribute to Deelip.com“.
Reader Mark Flayler pointed out a neat feature about Inventor’s sketcher that I didn’t know about. Apparently, while sketching you can enter something like “Length=50mm” in the in-canvas display and Inventor will automatically create a parameter called Length. Subsequently when sketching the next segment you can enter “Breadth=Length/2″ and another parameter called Breadth will be created. I have yet to start using this technique but it looks like a nice feature to have and use when you feel like.
I just did a quick check on the other modelers compared here. SolidWorks allows you to enter “Length=50″ in its in-canvas edit box but does not create a variable called “Length”. It simply strips out the non-numerical part of the text entered by the user and creates a dimension “D1″ or something. Solid Edge and Alibre Design do not allow non-numeric input at all. As far as Pro/ENGINEER is concerned, it appears that you cannot enter anything anywhere anyways.
If I have missed or overlooked something let me know.