Quick and Accurate Sketching

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.

Update:

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.

Update:

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“.

Update:

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.

  • http://twitter.com/SeanDotson Sean Dotson

    My comments on the new Inventor Heads Up display.

    http://www.mcadforums.com/forums/viewtopic.php?…

  • deelip_reader

    i couldn't watch the videos, but ProE has this functionality and it is enabled by default. (intent manager)

  • http://www.solidmastermind.com/ Jon Sutcliffe

    Just a quick note on Solid Edge to clear a couple of things up……

    It does have an auto dimension option. This will work in 2 ways, the first is that linear and angular dimensions will be added for all geometry drawn, even if values are not keyed in. The other (more preferred way) is to add dimensions when geometry is created with keyed in values. In the video you showed this would have been the option you wanted and all your dimensions would have been created.

    The option is activated by hitting the IntelliSketch command on the sketching ribbon.

    Solid Edge has had this capability for years :-)

    Also with regards to the Smart Dimension command. This is very versatile and WILL create angular dimensions as well as linear dimensions. In your video when you selected the two non-colinear lines, you could have hit the A key to create an angle dimension. Alternatively the toggle for this is in the left hand side command bar.

    Hope that helps
    Jon

  • http://www.deelip.com Deelip Menezes

    Whatever this intent manager is, it is definitely not enabled by default. At least not in my wildfire 5.0. Searched for it in the Pro/E documentations, found a lot of references to it in the help for the options variables but no way to activate it. Found a lot of people talking about intent manager on the internet. So yes, it is there and seems to do what Inventor and Alibre Design does. Now if I could only find a way to get it enabled.

  • http://www.deelip.com Deelip Menezes

    Thanks for the clarification. But I still need to move my focus from the left panel to the graphics windows over and over again, which is irritating. I'd prefer to do it the old way – create a rough sketch and then dimension in place like how I did in the video. The whole point here is to sketch effortlessly and seamlessly. That’s what Inventor's Direct Manipulation mini-toolbar is all about. You can completely do away with the parameters dialog box and work in the graphics windows only.

  • http://www.solidmastermind.com/ Jon Sutcliffe

    No problem Deelip, I agree having everything in the heads up display would prove more useful in Solid Edge….

  • http://www.marco-portfolio.blogspot.com/ Marco Savary

    Intent Manager is on all the time since version Pro20 way back in 1998. You have to turn it off by as an pull down menu command. The sketches are fully dimensioned and never over dimensioned.

    One of the week points of Intent Manager is, if you had too many lines it would slow down.

    But ProE feature base modeling mantra says: Keep your sketches as simple as possible. With many core machines the intent manager does a better job now.

    New users hits the wall in ProE when they want to sketch all the features at once!

    The inventor sketcher emulate ProE a lot, so you should try again or reinstall ProE and post the results.

    Do bench mark sketching a hexagon, dodecagon or something with a lot angles dimensions, arcs and lines.

    After using ProE for 12 years and all the CADs above. I can say that ProE is not a joke, but ProE out of the box is not very friendly for new users. You need to set it up well but it takes work. ProE is not one size fits all. ProE is very customizable.
    If you or anyone needs help setting up ProE config.pro and config.win, so you can get the most of it, let me know.

  • http://www.deelip.com Deelip Menezes

    Marco,

    Hell no, Pro/E is not a joke. But in the year 2010 its options box most definitely is.

    Maybe you didn’t understand my point. Say I start a sketch in Pro/E, I create a closed polygon by clicking away in the graphics window. I end up with a sketch that is all dimensioned and everything. That is not the point here. That sketch is far from accurate because I simply clicked away in the graphics window at locations that I thought were approximate to where the final locations will be. I then need to double click the dimensions and edit them.

    What Alibre Design and Inventor are doing is something totally different. You don’t need to click around anymore. You can specify the lengths of line segments or angles as you are sketching (as can be seen in my videos). Is that something the Intent Manager can do? If so, please create a video and upload it to YouTube of similar (or send it to me) and I will update this post with it.

    Another thing. I cannot find a way to sketch a polygon in Pro/ENGINEER. I have searched everywhere. I have read on some forums that Pro/ENGINEER does not have a polygon sketch command. I find that hard to believe since each and every CAD system I know can sketch a polygon. Can you help me here?

  • Alessandro

    What IV2011 does, SW makes from SW2009.
    Add dimensions when you sketch it's an option.
    Design Intent of Pro-E, no CAD has it.
    You have to use it and it's the best in class for parametric sketch.

    I have the impression that the information you writes .. are biased and incomplete because of a little knowledge of other CAD.
    I read the other post about the IV2011 and you can't compare Instant3D with Direct Manipulation which is superior, both on recalculation time and user iteration.

  • http://www.marco-portfolio.blogspot.com/ Marco Savary

    Dear Deeplip,

    I agree that in 2010 ProE out the box sucks, because PTC does have a wizard to deal with config.pro

    Well, well back to the post.
    I understand better what you are trying to compare.
    It appears that your ProE Intent Manager is working as it should.

    ProE Intent Manager functionality:
    A closed loop shape is always fully dimensioned and constrained all the time with called “Week Dimensions” on Gray color.

    Why is that way?
    It saves you time, so you can get out of the sketcher faster and see your results.
    You can select all dimensions or one by one. But is never over or under dimensioned.

    But why is that way?
    Because features regenerate faster.
    Complex sketches with many entities do cause havoc on large parts and assemblies.

    ProE feature based philosophy:
    A part with 100 features with simple sketches are better than a part with 1 super feature with 100 lines, angle dimensions, arcs and circles.
    Sketches shawl not have more than 6 entities… or something like that!

    In a summary:
    ProE does not prompt you to input a value as you sketch a profile. Is that bad!?

    My bias opinion:
    Intent Manager is 12-year-old now and constantly being upgraded.

    You can size your sketch correctly when your geometry is proven to be robust.

    If you like to be stopped by the software to input a value as you draw a line is a gage of good sketcher, you will not be happy with ProE Intent Manager. But it would be nice to have both ways.

    I will post something as soon I fix my Cad station.
    Nice article.

  • http://www.deelip.com Deelip Menezes

    Marco: “ProE does not prompt you to input a value as you sketch a profile. Is that bad!?”

    No, but it does not even show you lengths and angles as you sketch. Don’t you think it would be better to show you the distance and angle as you move the mouse cursor around in the graphics window? The only visual feedback that you get is a H or L letter telling you that the line you are drawing is horizontal or vertical. Which is almost redundant because the mouse cursor has already snapped to the horizontal and vertical and you already know that. Or maybe there is some cryptic option hidden somewhere that makes Pro/ENGINEER show lengths and angles. Enlighten me.

    BTW, you are not forced to enter a value for distance and angle in Alibre Design and Inventor. You are free to sketch approximately and no dimensions will be created. If you don't enter values are you sketch you at least have feedback (in terms of length and angles) of how close to the intended sketch you are. But if you do then it implies that you know exactly how much you want that length/angle to be and the software automatically creates a dimension for it.

  • http://www.deelip.com Deelip Menezes

    Alessandro: “What IV2011 does, SW makes from SW2009. Add dimensions when you sketch it's an option.”

  • danlanigan

    RE: Solid Edge

    I assume by moving your focus you mean your gaze must shift and not that the keyboard focus must be manually switched (e.g. with a mouse click). The keyboard focus is automatic.

    RE: SolidWorks

    As mentioned by Allessandro SW also has an auto dimension option. I agree that your article is misleading due to a lack of knowledge/research of all of the CAD packages mentioned.

  • http://www.deelip.com Deelip Menezes

    Dan,

    Regarding Solid Edge, yes keyboard focus stays with the edit boxes. It’s the human gaze that needs to shift every now and then. Try doing this for a long time and you are going to end up with a headache. The whole point of this head's up display and putting controls directly in the graphics window is to reduce strain on the human.

    Regarding SolidWorks, as I asked Allesandro, can you point me to the SolidWorks option that creates dimensions automatically if you enter a value for length (I know that Solidworks does not let you enter angles). Or are you both referring to the “Fully Define Sketch” command of SolidWorks, which appears to be the same as Pro/E's Intent Manager which this whole discussion is not about.

  • danlanigan

    Not sure about Pro-E, try this in SW:

    Toggle 'Enable on screen numeric input on entity creation' on, under options > sketch. While in the sketch environment toggle 'Add dimensions' on, under the options tab on the LHS panel.

  • http://www.deelip.com Deelip Menezes

    Dan,

    Thanks. I just posted this update.

    Update: 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.

  • http://www.deelip.com Deelip Menezes

    Alessandro: “What IV2011 does, SW makes from SW2009. Add dimensions when you sketch it's an option.”

    >>> Does SolidWorks 2009 automatically create a length dimension if you enter a value in the edit box in the graphics window as you sketch a line? I searched for an option to enable that but could not find one. Can you point it out to me.

    Allesandro: “Design Intent of Pro-E, no CAD has it. You have to use it and it's the best in class for parametric sketch.”

    >>> SolidWorks has an option to fully define Sketch. Basically you sketch around as you please and then right click -> Full define and all sketch elements are dimensioned and constrained so that the sketch is fully defined, which is basically what the Intent Manager of Pro/E does. Intent Manager in Pro/E is a very good thing. No doubt about that. I just think that it can be improved by giving more meaningful feedback.

    Allesandro: “I have the impression that the information you writes .. are biased and incomplete because of a little knowledge of other CAD.”

    >>> That’s precisely the reason why I am having this discussion with you. To learn from experts.

    Allesandro: “I read the other post about the IV2011 and you can't compare Instant3D with Direct Manipulation which is superior, both on recalculation time and user iteration.”

    >>> Not sure I got this right. Which do you think is superior? Instant3D or Direct Manipulation? Just so that you know, Instant3D in SolidWorks 2010 will not allow you to adjust the taper angle using the mouse in the graphics window like how I did using Direct Manipulation in Inventor 2011.

  • fcsuper

    Presumably, angles are derivative of two linear dimensions anyway. Either way, sounds like simple Enhancement Request to add angles; so that Autodesk (having finally caught up with other CAD systems) can again claim to be barely on par with the others.

  • Anonymous

    One thing that I haven’t seen mentioned here that I find helpful is creating relations between dimensions in Inventor. I mostly use this for equal dimensions. If you have an existing dimension that you have added for a sketch entity, when you add a dimension to another sketch entity you can click on one of the dimesions in your sketch that you want that entity to be equal to. Inventor will add an (fx) in front of the dimension to let you know that there is a relation between that dimension and another dimension in the sketch.

    I don’t remember if the other modelers do this or not.

    http://screencast.com/t/MWJjYjE4NmYt

  • http://twitter.com/Marijn1 Marijn

    Wasn't the whole point of this blogpost that it does this:
    In a summary:
    ProE does not prompt you to input a value as you sketch a profile. Is that bad!?

    If it is bad or not it doesn't matter. And you can screw up as much in pro/e as in any other cad program. If you want me to start pro/e bashing I can go on a lot longer. But it's off-topic.

  • danlanigan

    Deelip,

    Seeing as though you have updated the body of your post to report correctly about SW I figure Jon Sutcliffe's coments about SE should also be incoporated, fair is fair – don't you think?

  • http://www.deelip.com Deelip Menezes

    Marijn,

    You are correct. A lot to the discussion in these comments is off-topic. The topic here is a comparison of the ability and usability of sketchers that offer automatic accurate creation of length and angular dimensions while sketching curves in the graphics window. As far as I can tell, Pro/ENGINEER does not offer that. If you can enlighten me to the contrary it would be nice. The topic is not about the automatic constraining feature of Pro/ENGINEER (intent manager) or that of SolidWorks (fully define sketch command) or similar features that other CAD systems may or may not have. A comparison of those can be the topic of another post and discussion.

    Just to be sure the topic is “automatic accurate creation of length and angular dimensions while sketching curves in the graphics window” which is summarized by the title of this post “Quick and Accurate Sketching” and is shown in the embedded videos.

  • http://blogs.rand.com/manufacturing/ mflayler

    One other nice thing to point out about the Inventor Sketcher is that you can also rename the values as you typing them in the dynamic input and the name of that parameter updates. You can then use the named parameters throughout the modeling very easily by listing them onscreen. For instance in the video above, when Deelip is drawing the first 50 mm line he could type Length=50 mm and then the second line he could type HT=Length/2 then and continue using these values without having to open the parameters box. Fast forward to the part modeling, he could then use the right arrow box on the Direct Input to call those named parameters forward again whenever he wants them. Parameters and equations I have found to be much easier to access in Inventor than other packages. And this is out of the box, no configuring, no options in boxes to set, no cursor movement to left or right sides of the screen, there are a lot of professionals chiming in, but if Deelip even didn't know about it take a look at any other casual user of the software and see if they knew that either.

    I would like to see a continuation of this thread to actually show more design intent dealing with equations or parameters as well as a look at the other Auto Define options in the other programs. Personally I never use the Auto Dimension command in Inventor because the computer does the thinking for me and is usually wrong in my intent.

    Something SW could learn from to be on par with Autodesk. Forgive the last statement, all software discussed here have their advantages and shortcomings, what I like about the Autodesk solution is that is more well rounded and integrated with their other products. What I truly like is the more uniform appearance, interface, and materials across all their products now so it is easy for someone who knows AutoCAD or Revit to play in the Inventor sandbox make an Accumulator and then take it to Revit with all the correct materials and metadata and the correct hookups already assigned for the MEP.

  • http://www.deelip.com Deelip Menezes

    Just did.

    Update: 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.

  • http://www.deelip.com Deelip Menezes

    Mark,

    No, I didn't know that. Thanks for pointing it out here. That is really a nice feature.

    I just did a quick check on the other modelers compared here. SolidWorks allows you to enter “Length=50″ in the edit box but does not create a variable called “Length”. It simplly 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, you cannot enter anything anywhere anyways.

  • http://www.deelip.com Deelip Menezes

    Updated the post to mention the enhancement in Inventor's sketcher that Mark Flayler pointed out.

  • fcsuper

    Yup, SolidWorks requires a separate action to input formula. That would outside the scope of this posting, but it is a good point.

  • http://twitter.com/robcohee Rob Cohee

    What I get from this discussion isn't that the other CAD applications don't have this functionality, its that it isn't as integrated into the sketching commands as it is with Inventor 2011. Yes, you can name parameters, yes you can do auto, gyro, uber constraints, and yes you can do most of the things independently, or as a separate set of commands. The point as I see it is that sketching, dimensioning, parameter management and referencing all occur within a single command in Inventor 2011. The user can choose which ones they want to use, or ignore them completely and it has no effect on the usability or user experience.

    Great discussion guys.

  • http://twitter.com/ProphetPVD Jay Tedeschi

    One aspect of the heads up dimensioning that I think is easily overlooked is the ability to “lock” values for distance or angle and then drag the other value. For example, in the video, when Deelip adds the fourth segment, he enters a value of 135 degrees. This keyed entry is locked, and in this instance he is then free to drag any distance value at that set angle. Very nice and as I pointed out on Sean's McadForum's it allows you to create a sketch which is much closer in proportion to that which the user envisions, which helps greatly in creating sketches that accept change without distortion.

    As far as parameter naming is concerned, it's a very nice feature, but it has not drastically changed the way that I model… heads up dimensioning has.

  • Marco Savary

    Deelip,

    There is no preview or any virtual ruler to guide you on the sketcher and no config.pro as far I know.
    You eye ball a closed or open profile and then you size it correctly after.

    Yes I do think that dynamic dims preview is a missing feature and I hope that PTC will implement that in a future release.

    But there are few more things that PTC has to improve before on the sketcher environment.
    -The sketcher zoom defaults at a large scale around 800 units or so. So when you think you have eye balled a 4″ circle you end up with a much larger circle, around 400 inches depending of your zoom state.

    Deelip for predefine shapes like a Heptagon, try this pull down menu. Sketch/Data from a file/Pallet, or the funny looking ameba shape icon next to the big A icon.

    So in a feature-by-feature comparison, it is a thumbs down to ProE sketcher.

  • Alessandro

    You have write that SolidWorks can enter only lengths and not angles.
    This is not true.
    You have to set the last option (angle) when you sketch line.
    Another mistake.
    Inventor is a follower CAD.
    IV2011 has functionality that other CAD have 2 or 3 years ago.
    Please make some simple test on the Fusion Preview.
    It works very bad.

  • http://blogs.rand.com/manufacturing/ mflayler

    How is Inventor a follower product if they clearly are the winner in this area. It is true they played catch up for a while a couple releases ago but around Inventor R11/2008 it really struck out on its own. Inventor also has technology that other CAD will or will not have for 2 or 3 years. Fact.

    Fusion is a technology preview, not an RTM product and NO ONE is doing it the way Autodesk is. Again this is another topic. Deelip did a very extensive covering of Fusion TP2 and I expect that he will have a nice write up on TP3. How is SW doing on that front? Oh yea, that's right, they dismissed the technology as gimmicky or non nonsensical until they previewed something similar at SWW. Have you tried the Technology Preview 3 with the Change Manager for Inventor? Have you provided feedback on what you would want in Fusion?

    SolidWorks follows Inventor as much as it is the other way around. The End of Part marker…Inventor first; Dual Dims in Hole Tables…Inventor first, many more could be said back and forth. I think you can agree though that in this area the SW method is not user friendly enough or not understood as easily enough as numerous SW have chimed in here and not found the option you speak of yet. I am sure SW will add this soon enough though…following Inventor and all :)

  • http://www.deelip.com Deelip Menezes

    No, it is not a mistake. In SolidWorks, the length and angle edit boxes in the LHS panel cannot be edited while you are sketching. After you finish sketching you can select segment and then change the values for length and angle. That is not what is being discussed here. As I wrote in the update, while sketching you can only enter lengths in the graphics window, not angles.

    Fusion is anything but an example of “follower CAD”. Yes, they are still fixing and tweaking it. But as far as I know, no other CAD vendor has tried to do what they are doing.

    It would be helpful not to have preconceived notions about CAD systems and their makers and look at things with an open mind.

  • Alessandro

    It's a mistake.
    In SolidWorks, the length and angle edit boxes in the LHS panel can be edited while you are sketching.
    Maybe you are installed SW for the first time and you don't know how to use.

    Fusion has big problem with simple modified part.
    Anyway I prefer solution of direct editing with chronology feature or Instant3D

  • R.H. (Rick) Mason

    Deelip,

    As a veteran parametric 3D user and a user of Solid Edge since Version 1.0, I can't argue with your point about having to continually shift focus from the sidebar menu etc. to the sketch geometry. What I will say is that NO 'auto-dimensioning' sketcher which I have used applies the SCHEME of dimensioning that I need, to ensure that the sketch geometry is 'driven' precisely as I require. Often it is important that certain offsets, datums etc. are maintained which are not obvious (or, necessarily, simple!) hence my preference is to create an approximate profile with the correct geometric constraints, then progressively apply the specific scheme of dimensioning that is required to correctly & robustly control the profile about its origin and references. Dynamically adjusting these dimensions to achieve the final result is itself a test of the robustness of the sketched profile, hence highly valuable. Simply auto-dimensioning a sketch doesn't test the dynamic behavio(u)r or integrity of the profile, and (in my experience) results in a poorer result.

  • http://www.deelip.com Deelip Menezes

    Are you suggesting that Pro/ENGINEER's Intent Manager gives poor results? It auto dimensions and constrains as the user draws a rough sketch and then lets him tweak the dimensions later on. And apparently now you cannot even turn it off. Like you I prefer to dimension my sketches myself.

    In Alibre Design and Inventor, it is not mandatory to dimension the sketch elements as you proceed drawing them. But if you feel like it then the option is there. For example, if you are sketching a circle and you know that you will want to dimension it later and create an equation for it, you can directly enter “Inner_Radius=10″ and a parameter will be automatically set up for you. I think having such a feature is better than not having one, especially if it is completely optional to use.

  • R.H. (Rick) Mason

    I have no experience of Intent Manager – my experience with Pro/E stopped with 2000i^2. As to the merits of fully-dimensioned sketches, this a vexed question. Is the sketch preserved/linked, or consumed/discarded? From a checker's perspective, a well-dimensioned (and associative) Sketch profile is godsend. Much of the dialog(ue)/hype about History-free modeling ignores the basic need to CHECK the geometry which has been created – but that's a topic for another day!

  • http://www.deelip.com Deelip Menezes

    Alessandro,

    I just rechecked, this time very carefully, and now see what you mean. That SolidWorks option is a joke. As you are move the mouse the edit boxes for length and angle are disabled. You need to click the mouse somewhere and then not move it at all. Only then will you be able to edit the values for length and angle. If you move the mouse the edit boxes become disabled again and you do not get a chance to change the values that were there previously. This is practically unusable and by far the most idiotic implementation I have ever come across. Try using it yourself and you will see what I mean.

  • http://www.deelip.com Deelip Menezes

    Are you suggesting that Pro/ENGINEER's Intent Manager gives poor results? It auto dimensions and constrains as the user draws a rough sketch and then lets him tweak the dimensions later on. And now you cannot even turn it off.

    In Alibre Design and Inventor, it is not mandatory to dimension the sketch elements as you proceed drawing them. But it you feel like it then the option is there. For example, if you are sketching a circle and you know that you will want to dimension it later and create an equation for it, you can directly enter “Inner_Radius=10″ and a parameter will be automatically set up for you. I think having such a feature is better than not having one, especially if it is completely optional to use.

  • Mike Robbins

    When a feature (like keying-in length and angle while sketching)does exist, there is no clearer evidence that this feature is poorly designed if a bright, intelligent user (as Deelip appears to be) BELIEVES the feature does not exist. Difficult to discover features are not user shortcomings, they are product design shortcomings.

  • donbreda

    Hi Deelip,
    I saw your blog and wanted to answer your questions regarding Pro/ENGINEER. I just wanted to confirm for you that you are correct, there is no way to receive dimensional feedback while creating sketched entities, or to be prompted for an input value as you sketch a profile in the current release of Pro/ENGINEER.

    Pro/ENGINEER follows the philosophy that the user should define the profile based on his design intent, but that the software should help the user to get there. As you know, in Pro/ENGINEER, the user first provides a rough, relative sketch of the desired profile. As the user sketches their profile, the software automatically provides constraints and dimensions for an initial dimensioning scheme. The user can then modify this dimensioning / constraining scheme to reflect his final design intent.

    PTC has streamlined the sketching workflows to make them faster and more efficient in recent releases. These improvements include: right mouse button access in the graphics window to refine sketch setup and references; prompts for dimension values while defining the dimensioning scheme; and object action workflows for constraints (pick one or more entities in the graphics window, and the right mouse button menu will offer the user only applicable constraints).

    In reference to your question about creating polygons in Pro/ENGINEER Sketcher, they are located in the Sketcher Palette, along with many other PTC provided, and user defined, profiles and shapes.

    In reference to entering non-numeric input for dimension values, Pro/ENGINEER allows you to directly enter an existing parameter name or expression into a dimension value prompt (Length/2 for example). This will automatically create a relation for that dimension value. Also, since all dimensions in Pro/ENGINEER are automatically assigned a parameter alias (#Info > #Switch Dimensions to see these), it is very easy to relate a dimension value to any other dimension value.

    Thank you very much for your informative blog Deelip. For more details or additional questions on Sketcher in Pro/ENGINEER, please email me.

    Don

  • http://www.deelip.com Deelip Menezes

    Don,

    Thanks for stopping by and leaving a detailed comment.

  • Alessandro

    I'm sorry but I don't have your problems.
    Anyway I wrote to you because you wrote inaccuracy on SolidWorks.
    Like all CAD systems should be improved.
    Improvements come from customers and probably none use these features because they prefer to dimension the sketch as they wish.
    I am one of them.
    Honestly I never used.

  • duartemv

    Also, this option is available since SW2009. It was one of the many novelties of that major version (page 29 of the What's New pdf file that comes with the software).

  • Tanzil_mirza

    i wanna tapper 




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