Partially Disable Sketch Auto-Constraints

[Anonymous]

Hello

I'm using Inventor 2016.

I am currently working on a project that requires sketches to have a considerable amount of geometry on them. While working on a sketch, I don't want Inventor to assume where I want constraints.

So I found out how to switch that off reading this thread:

https://forums.autodesk.com/t5/inventor-forum/please-stop-automatic-constraints/td-p/6937031

And I disabled the annoying behavior. Unfortunately however, this created another issue:

The rectangles made with the rectangle tool are no longer constrained either. Which means that I can select a vertex, drag it and pretty much end up with a four sided polygon I have absolutely no use for.

To disable the auto-constrain feature, I went to Inventor, Options, Sketch, 2D Sketch, Constraint Settings, Inference and unchecked the Infer Constraints checkbox.

If I need to draw several rectangles on the same sketch, each having different dimensions and positions, I would like the rectangles to keep their inner constraints (parallel edges and 90° angles) but not automatically set co-linearity constraints between the individual rectangles. It's very often that I find myself setting dimensions between a side of a rectangle and another element and then notice that another rectangle on the sketch decided of its own volition to tag along and exhibit the same behavior. I know, constraints can be removed and so on and so forth. But I don't really want to have to edit constraints for every single sketch in order to make sure that Inventor does not mess up my geometry. I am quite fed up with having to delete geometry over and over again because of these auto-constraints yet at the same time, I expect a rectangle to remain a rectangle.

Is there a way to achieve this?

Thank you for your help.

[mcgyvr]

I don't think you can pick and choose which constraints get inferred and which do not..

But have you tried enabling "relax mode"..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2015...

[Anonymous]

Hey McGyvr,

thank you for your reply.

About "relax mode", it does sound interesting but I think that it won't help me much because:

" By default the following will not be changed with Relax Mode ON:
    Coincident, Tangent, Symmetric, and Smooth constraints.
    Dimensions controlled by equations.
    You can change the default behavior in the Constraints Settings dialog box in the Relax Mode tab."

The trouble is that the rectangles created by the rectangle tool are defined by four parallel constraints, one horizontal and one perpendicular constraint. Which in essence means that the behavior of the "relaxed mode" would be the very same as with inference off, which in turn forces me to dimension and/or constrain every rectangle the rectangle tool makes, which in turn (yes, I do like turns), means that the rectangle tool becomes obsolete.

On the other hand, if I do not alter the way constraints are applied, it means that whenever my sketch contains more than one geometric feature (and that is normally the case), the inference on feature causes the vertexes of separate rectangles to latch on to either the vertexes or the center points of unrelated rectangles. Which would not be a problem if these inferred relationships could actually be overridden by the user applying actual constraints manually.

In essence it causes me to either delete already drawn geometry or to actually draw one geometric figure at a time, constrain it, then add the next and so on, which is a highly inefficient workflow due to the fact that it forces the user to incessantly switch between the tools.

To be clear:

I need three rectangles on my sketch, each constrained to fixed positions related to geometry outside the sketch.

The efficient way to do this is:
Select rectangle tool, draw three rectangles randomly on the sketch, select horizontal constraint, apply it to all three rectangles, select vertical constraint, apply it to all rectangles.
(As already mentioned, the downside is that if Inventor decides to randomly infer constraints, it means that the user in effect cannot constrain the rectangles without deleting at least one of them)

The Inventor way of doing it:
Select rectangle tool, draw rectangle, select horizontal constrain, apply it, select vertical constrain, apply it.
Repeat this for each of your three rectangles.

Doesn't this simply create unnecessary clicking?

Which would be fine, if people were paid per click. Unfortunately they are paid for finished projects and clicking takes time 🙂

[JDMather]

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@Anonymous wrote:

...

Which would be fine, if people were paid per click. Unfortunately they are paid for finished projects and clicking takes time 🙂

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If you can attach your finished part here (using whatever number of clicks it takes) I would like to take a shot at seeing if I could come up with a more efficient technique.

[mflayler]

Have you tried holding down CTRL while sketching.  That should disable most of the inferred constraints.

[EvanGu]

In Constraint Settings, Inference tab, clear the constraints you don't want, see attached snapshot.

[Anonymous]

Hello JD,

thank you for your reply.

The issue isn't with a particular part, it's with every single sketch that needs more than one feature.
I have just made a new example of what I mean. The sketches that control all the holes for dowels and for the hidden dovetail joint at the bottom are all a pain to work with because of the constraints.

It's not too bad working with circles because circles are I think defined differently and do not require geometric constraints to retain their shape. Nor do they change shape when you drag them around.

The trouble with the constraints is when using rectangles, other types of polygons or when creating a closed loop with the line tool - dovetails are symmetrical trapezes, so I have to draw a random loop, parallel the bases to each other, constrain the centers of the bases to each other, then enter values for the two bases and for the distance between the bases and then use a collinear constraint to constrain them to the edge where the join will appear.

Because of the way the inference works, I end up with some constraints that, when I enter a dimension for one of the bases, it skews the other figures as well, sometime moves the while geometry far away from the spot where I drew it on the sketch and other weird behaviors.

I am aware, I could just make one of the shapes and then copy it. But when it comes to Inventor, I do not like how the copy function works. I select geometry, I click on the copy button, then I have to select a basis point and then eventually, the copying occurs. It's not nearly as base with ctrl+c ctrl+v commands but I don't like the way constraints are copied because... well because I am a control freak and I like to do the constraints myself rather than rely on a program to do it for me. And for me at least it is simpler to place constraints precisely where I want them, rather than to edit constraints with F8 and then delete the ones that I didn't want to begin with but the program wanted me to have.

I know, my way of doing things is most likely not the best way to do it, I am sure that my way of doing things is not streamlined to fit with Inventor. But at the same time, some of the things Inventor does defy common sense and to compensate for that I make up my own sense.

If you remember, one of the first things I said when I came to this forum about a year ago was that I hate constraints.  still  hate them even now, but I can now see that they are necessary and they are quite helpful when using a lot of parameters (I use those heavily - just not in the example I posted simply because it's merely an example and I didn't have the time to sit down and suss out which parameters make sense). But I do want to actually use the constraints myself. 🙂

I'm sorry if I'm a bit daft that way.

Thank you for your help 🙂

[Anonymous]

Hi Mark,

thank you for your reply.

Nope I haven't done that and it does indeed solve the issue. Partially. I sketch a lot. Just look in the example I posted for JD so you get an idea about that. Holding ctrl down do disable a functionality that is imposed upon me is going to give me a very sore finger at the end of the day. If anything, I would accept it if it were the other way around, turn of the inference and hold down ctrl when I actually want it - which would be never.

So yes, you have given me a solution and I thank you for that. But I do not believe that I will often use it. It's just too counter-intuitive.

Many thanks again 🙂

[Anonymous]

Hello Evan,

thank you for your post.

I have looked at those constraints yesterday and I decided that it's not worth fiddling with for a very simple reason:

When using the rectangle tool, the rectangle is defined by parallel, horizontal/vertical and perpendicular constraints. Those are the very same inferences that I wish to turn off so that Inventor stops bungling up my geometry. If I do disable them, my geometry will no longer be messed up but my rectangles would. So not really a way to go, I think.

Thank you for your help.

[JDMather]

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@Anonymous wrote:

.... I hate constraints.  still  hate them even now, ...

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Is it too late to change majors?

I see a lot of duplication of work.

I am lazy - I try to avoid unnecessary work.

Are you familiar with Sketch Blocks and/or iFeatures?

[Anonymous]

There are some timesavers possible.

I wouldn't turn constraint inference off, that's many bridges too far. The very least we want is connected lines and arcs since every feature relies on it.

As mentioned the CTRL key is a golden key to allow the user to apply intelligent constraints afterwards. And it keeps lines connected.

In application options you have a priority setting that will effect rectangles, either orthogonal or parallel and perpendicular. Take your advantage of it.

When drawing rectangles you can choose the 3-point rectangle as default if you want to avoid horizontal and vertical constraints being set in the background. The rectangle stays rotated until you connect it to geometry defining orientation.

Keep sketches simple. Undesired autoconstraints are more likely when IV finds lots of elements to relate to.

Alex

[Anonymous]

Hey JD,

thank you for your reply.

It's never too late to change majors. I just did switch to technical design :). But me hating constraints is one thing. I am using them and I can see their usefulness. Sort of 🙂 At any rate, I am seldom leaving sketches unconstrained because I have seen what happens when you do and it's not pretty.

And yes, it is a lot of duplication of work and I am lazy as well and I would rather not duplicate work but I'm afraid I don't know how to avoid that. The only Inventor "training" I got was a manual that shallowly explained the very basic use of the program and didn't even come as far as the concept of a mirror, the basics of an assembly (how to constrain parts and how to enable contact) and the basics of a drawing.

Everything else I know I have learned by doing: find out what I want to do, think how I would do it in SketchUp, see how Inventor does it, fail, look up threads in this forum to find out what I'm doing wrong. Thus, in essence, the people on this forum have taught me quite a lot of what I now know about Inventor. I might be stubborn and it may appear that I am not listening, but I actually am.

As for Sketch Blocks and/or iFeatures. Nope, I'm not familiar with them. Blocks I have seen used in my 2 weeks of Autocad immersion at the beginning of my education. I know there are blocks and web blocks and that they do come in very handy. But I have not seen them mentioned before in Inventor. In SketchUp, since it does not have the concept of a sketch or even part files and assemblies, I use components (the SketchUp version of a block) a lot, in order to separate geometry into bits I can work with and make sure that they do not interfere with the rest of my work.

I would love to learn about Sketch Blocks and/or iFeatures, it's just that in the first 6 months of the education we've had projects non-stop, all on a deadline and I didn't have time to try to understand what I was doing, I simply did everything best I could. In the end, the knowledge of Inventor is not important (to me it really is because it's a very powerful tool and I'm sure it can do a lot more than I can imagine at this point) as long as the drawings we produce are readable and understandable. I suspect that if I chose to draw the drawings by hand they would also be accepted.

Thus, if you could provide me with a link to a tutorial for Sketch Blocks and/or iFeatures (beginner level), I would definitely be more than happy to look into it.

Thank you for your help, JD (and everyone else). I really do appreciate you taking the time to teach a complete stranger.

[Anonymous]

Hello Alex,

thank you for your reply.

I tried turning off constraint inference off, but I didn't like the fact that it also turned off constraints for rectangles.

As Evan suggested, I have begun using the ctrl key and it works, it's just cumbersome and sometimes I forget it and realize it's been on only halfway through the sketch.

In Options, Sketch, Sketch, Constraints, Settings, Inference tab, there is indeed a list of all the constraints. Unfortunately, the very ones that I want turned off are the ones that I need for rectangles. Either that, or I am missing something.

My annoyance is that Inventor does not differentiate between geometry constraints it sets itself when creating a rectangle, a polygon, a line, a circle etc., the inference constraints it arbitrarily adds when the user creates geometry and the constraints the user applies. Correct me if I am wrong, but shouldn't the user added constraints supersede inference constraints? Geometry constraints should be fixed until the user manually removes them, user constraints should rule absolute and inference constraints should be the weakest of all sketch constraints because they are the result of Inventor "assuming" what the user wishes to do. Again I relate to SketchUp. It also uses inferences but it completely keeps them as a suggestion only: there the inference is only displayed when the user actually hovers over an inference point, otherwise the program does not infer anything. For example if I have a line and I draw another line, SketchUp will not assume any relation between the two until I hover with my mouse over the center or one of the two ends of the first line. Inventor assumes relationships and applies the relationships as soon as the cursor is vertically or horizontally aligned to centers, end points or vertexes. Not ok 😛

I will attempt to use the three point rectangle to see what happens with the inference.

As for keeping sketches simple, I am doing my best to but it's not always an option. When I create a solid, the sketch is simple. But when I need to put holes into a solid, I do need to have several points (or circles) on the sketch, otherwise I will end up with a lot more work. So yes, Inventor does find a lot of elements to relate to in my sketches and I do not know how to avoid having 5 holes in a sketch, when I need to have 5 holes in my solid that have to be aligned to each other so that I can set in dowels.

Many thanks for your help. 🙂

[EvanGu · Accepted solution]

Hi Kamiasahi,

Just clear some constraint types under Selection for Constraint Inference does not prevent to create the internal constraints (parallel, horizontal, vertical) of a rectangle. It looks like you turn off Persist constraints option as well.

[Anonymous]

Hello Evan,

Domo arigato gozaimasu.

That was definitely it. I turned off all the constrains from inference settings but left the "infer constraints" and "persist constraints" untouched and hooray, my rectangles remain rectangles now and even when I have two on the same sketch they no longer behave like they're married with children 😛

You have really made my life a LOT easier. Thank you again 🙂

[Bert_Bimmel]

Hello Everybody

I'd like to add that to me the nucleus of the problem is the change of behaviour with remote geometry. I'd swear in earlier versions of inventor, i could attach line endpoints to other geometry by clicking ON it...

... or by shortly hovering over my desired geometry to place a constraint on, and then pull my mouspointer along this geometry and click somewhere else:

This was a convenient solution, and it's still possible and I would like to maintain it.

BUT:

Since - i don't know -  Inventor started proposing (and applying) constraints to geometry that's far away from my mouspointer, and if there's already plenty of geometry in my sketch, the dashed lines indicating which constraint Inventor will apply upon click here get hyper nervous, and it's almost impossible to klick somewhere without applying any unwanted constraints:

Holding down ctrl is not a solution, as then, it will not apply ANY constraints other then end points even IF I click right onto the desired connection.

So to me, this was a classic "If it ain't broke, don't fix it!". At least not without giving me a chance to turn things back to "normal" in my constraints options.