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Help with getting to grips with Constraints

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Message 1 of 58
t_smith5
1851 Views, 57 Replies

Help with getting to grips with Constraints

Hi

 

I'm having some issues getting to grips with fully constraining a Sketch and I felt it was time I got on top of this. I understand that fully black lines/Sketches means it's fully constrained whereas the default blue isn't. That's pretty much what all of my Sketches are like. ๐Ÿ˜… So I'm going back through some of my Sketches and fixing them up as best I can for practise. I seem to be having some issues with a simple rectangle though, which is the foot/toe of my mech.

 

Is it fine to have shapes in a Sketch join up to others? Or is it recommended to have each shape in a Sketch a separate entity? The parts of the foot/leg I have do have areas where they're close or connected with a Coincident constraint. Also, is it possible to assign a different colour to each part/shape rather than using the default light blue?

 

For this rectangle, I've been experimenting with constraining it correctly, but the lines just won't turn black. Either that, or I end up getting an error saying it's 'over constrained'. I've tried to make sure all constraints that were there have been deleted and pulled the lines apart. But whether I try to connect the Sketch Points up with each other with a Coincident or Perpendicular constraint, I still get the error about it being over constrained. ๐Ÿ˜•

 

Are Sketch Dimensions considered to be constraints? This rectangle is 90cm in width and 40cm in height. I did try figuring out how to straighten the vertical lines and line up the horizontal ones, but haven't been able to. I thought maybe a constraint would help there...?

 

I've tried using a Coincident in each corner to join the Sketch Points up and then after that adding a Perpendicular in each corner. I can normally only add three before it says it's over constrained...? No matter what I do, the lines don't turn black. I've tried deleting the lines and adding new ones, but get the same issue if I specify the width and height.

 

This is with the regular Line tool, I should add. I suppose for this it would make sense to use the 2-point Rectangle, but just wanted to experiment with fixing constraints manually. When I have used the 2-point Rectangle tool though, the lines still don't turn black.

 

In the attachment, the problem area I've been playing around with is the rectangle in the bottom right corner.

 

Thanks

57 REPLIES 57
Message 2 of 58
jhackney1972
in reply to: t_smith5


@t_smith5 wrote:

 

 

Is it fine to have shapes in a Sketch join up to others? Or is it recommended to have each shape in a Sketch a separate entity?

This is dependent on your design needs.  I feel it is important to keep your sketches simple having multiple sketches to create your component bodies or add/subtract from them.

 

  Also, is it possible to assign a different colour to each part/shape rather than using the default light blue?

 

No, not at this time.  You can try different color environment color schemes.  In my case, I am using Grey Room where my fully constrained sketch lines turn white.

๐Ÿ˜•

 

Are Sketch Dimensions considered to be constraints? This rectangle is 90cm in width and 40cm in height. I did try figuring out how to straighten the vertical lines and line up the horizontal ones, but haven't been able to. I thought maybe a constraint would help there...?

 

Sketch dimensions are not sketch constrains but are a part of defining the size and/or location of the sketch which is a part of the sketch constraining process.  In the video you will see this.

 

 

 

 

 


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 3 of 58
Bunga777
in reply to: t_smith5

I took a video of how I added the restraints to the attached sketch to make it fully restrained.

I only made it halfway through, but you can see how I added dimensions and restraints to the necessary areas.

 

 

At the end of the blue line is a white point; drag this point to move it.

You can visually tell which constraint is missing by the way it moves.

So if you have trouble with a line not turning black, try dragging the white point.

If this causes your sketch to fall apart, you can quickly revert it with Ctrl+z.

 

As for splines, there is a knack for complete constraints, so it is best to have a complete understanding of the other constraints before starting on splines.

 

I hope you will find this video helpful in understanding the restraints.

Message 4 of 58
t_smith5
in reply to: jhackney1972

Hi

 

Thank you for the video. It looks like I was going about things correctly with the Coincidents and Horizontal/Vertical constraints etc. but the one thing I didn't know was needing to constrain it to the Origin. ๐Ÿ˜„

 

RE working in Centimetres: that's what I've been taught at my university (in the UK), particularly with software like 3ds Max and Maya for making game-ready assets. I'm not 100% sure on the reasoning. It's something I'll need to ask and look into. Plus, I've always used Centimetres when measuring things with tape measures etc. ๐Ÿ™‚

Message 5 of 58
TheCADWhisperer
in reply to: t_smith5


@t_smith5 wrote:

1. but the one thing I didn't know was needing to constrain it to the Origin. ๐Ÿ˜„

 

2. RE working in Centimetres: that's what I've been taught ...I'm not 100% sure on the reasoning.


1. I thought we covered this a month ago...

Is the BORN Technique starting to sink in now?

The Origin is your single source of truth (datum) in the design.

I recommend that beginners create only ONE line, circle or rectangle at a time and fully define position and size before moving to next line, circle or rectangle...

TheCADWhisperer_0-1681040852769.png

 

2.  Most design software uses cm in the background as native default units.  These days most software is units aware so you can specify any units and the software will convert for you in the background.

Message 6 of 58
t_smith5
in reply to: Bunga777

Thank you for this. ๐Ÿ™‚ Again, it looks like constraining to the Origin Point was the mistake I was making, for the most part. Your video is certainly helpful, however, having a voiceover explaining the reasonings behind some of the chosen constraints would have helped. I'm still a bit unsure why certain ones are needed and where they ought to go. ๐Ÿ˜… Also, with the amount of contraints and dimensions you added, I'm surprised it didn't throw up an error saying it was over constrained. ๐Ÿ˜‹

Message 7 of 58
t_smith5
in reply to: TheCADWhisperer


@TheCADWhisperer wrote:

@t_smith5 wrote:

1. but the one thing I didn't know was needing to constrain it to the Origin. ๐Ÿ˜„

 

2. RE working in Centimetres: that's what I've been taught ...I'm not 100% sure on the reasoning.


1. I thought we covered this a month ago...

Is the BORN Technique starting to sink in now?


Ah. I completely forgot about that detail. ๐Ÿ˜… But yeah, hopefully, it is. ๐Ÿ˜

Message 8 of 58
t_smith5
in reply to: t_smith5

So, does every line need to be constained to the Origin Point or is it the overall shape? And does it matter too much what Dimension needs to be set?

Message 9 of 58
t_smith5
in reply to: t_smith5

Also, I appear to have a random Sketch Point bang on the centre of the Origin Point. Is there any way of removing it?

Message 10 of 58
jhackney1972
in reply to: t_smith5

Normally the general sketch shape or group of entities.  A sketch rectangle consist of four entities, lines in this case, they are jointed together at their endpoints with Coincident sketch constraints.  The lines either have vertical or horizontal sketch constrains on them, if the rectangle is in line with one of the axis.  This is a group of entities.  If you either add sketch constrains between the rectangle and the origin or use dimensions to define its relationship to the world, the origin.

 

The answer to your second post is the white dot at the center of the Origin is the origin point.  Go to your browser and open the Origin for the assembly, in this case, and highlight the point you are looking at.  If not, you need to send along some screen captures to show what you are truly looking at.

 

Origin Point.jpg


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 11 of 58
t_smith5
in reply to: jhackney1972

I see. Thanks for the explanation.

 

As to the point in the Origin, there's definitely a Sketch Point 'embedded' in the centre of it. I'm guessing it's related to a part of the Sketch somewhere...? A constraint...?

 

Fusion360_oGY5yu6JMF.gif

 

I've attached my latest file. I've changed things up whilst practicing and improving it.

Message 12 of 58
jhackney1972
in reply to: t_smith5

Yes, there is a sketch point there but as you can see, it cannot be deleted unless you delete your entire sketch, and I am sure you do not want to do this.  It is probably related to another sketch entity in the remainder of the sketch.  Do not worry about it, move on.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 13 of 58
t_smith5
in reply to: t_smith5

Okay.

 

I seem to be struggling with getting these contraints when adding Sketch Dimensions to the Origin Point. ๐Ÿ˜• With this GIF I recorded, I don't tend to get any lines that you can position where you want the Sketch Dimensions to display.

 

Fusion360_96GGyWh9yq.gif

And I've attached the latest file...

 

I believe I'm approaching it right. Maybe...? I click on Sketch Dimensions, or press D, click on the Origin Point and then click on the needed line, but I don't appear to be getting the results I'm expecting.

Message 14 of 58
jhackney1972
in reply to: t_smith5

You need to turn off the canvas in the background so you can see the sketch.  It makes it a lot easier.  When you get to the spline, you will find trying to fully constrain it a bit more difficult.  I would constrain its location and then just Fix it.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 15 of 58
t_smith5
in reply to: jhackney1972

Okay, thanks for clearing that up. I'll turn off the Canvas and have another play around with it. ๐Ÿ™‚ Also, I didn't realise you could hold down the left mouse button to select from multiple objects. I've only ever seen a list of actions from using the Edit Feature.

Message 16 of 58
t_smith5
in reply to: jhackney1972

Actually, one thing I am confused about is that you managed to contrain the two smaller circles in one fell swoop by clicking on the Sketch Point for the centre ring and constrained it to the Origin Point with a width of 18. Both turned white. I've tried the same thing but neither circle turns black. I'm guessing it's due to needing to constrain something else first...?

 

EDIT: Yep. Answered my own question. ๐Ÿ˜… I needed to use to Coincident constraint to the bottom line and Origin Point.

Message 17 of 58
TheCADWhisperer
in reply to: t_smith5


@t_smith5 wrote:

So, does every line need to be constained to the Origin Point or is it the overall shape? And does it matter too much what Dimension needs to be set?


Dimensioning (and tolerancing) is a large topic that often is a college level class by itself.

 

There is Ordinate Dimensioning system where every position is dimensioned to the Origin, but this has some limitations related to assembly and functionality of the features.

 

Many companies have moved to the Geometric Dimensioning and Tolerancing system (GD&T) and beyond that to Digital Product Definition (by various names).  Search Wikipedia on these.

 

In general I am going to suggest that you pick a Primary, Secondary and Tertiary datum for your geometry.

Locate the Primary datum at the Origin.  For cylindrical parts or things that rotate about an axis this is self evident.

For other geometry shapes this might be based on function or manufacturing process set-up.  In CAD we often pick an imaginary location of symmetry left to right and/or top to bottom.  Even partial symmetry.  As this aides in simplifying modeling.

 

Understand that we cannot manufacture perfect parts - every feature has size and position dimensions and every dimension has an associated tolerance.  For example if we have a hole located 10mm in both x and y from the Origin we cannot actually manufacture exactly 10mm in both x and y from the origin.  This starts to become a very very complex topic with understanding and experience with manufacturing processes and assembly and actual function.

In general you want to design with a strategy that the largest possible tolerance will still result in a functioning assembly.  Beginners often get this backwards as they want perfect parts or tight tolerances to ensure that everything goes together and works.  Specifying tight tolerances is fine - but with every reduction in tolerance you increase the cost of the feature and risk more scrap. 

 

I would say that as you pick your datums consider if a dimension is off a bit (in manufacture) what is important and what is not so important to assembly/function.  And if you edit dimensions (editing is always required - nobody gets everything right the first time - that is the power of parametric design) the sketch/features update predictably, reliably and robust with no errors or yellow or red highlighted issues in the Timeline.

 

I am flabbergasted that  every year at Autodesk University - the premier showcase of Autodesk products - that in the mainstage Keynote presentation they will have a Fusion slide in their presentation with a Timeline full of unresolved issues highlighted in yellow and red.  This is the geometric equivalent of having a slide with spelling and grammar errors that were pointed out by PowerPoint (or whatever software).  Do not ignore issues.  As I typed this I made several spelling errors.  The forum interface let me know and it was easy to fix.  Do not leave highlighted issues unresolved.  That is just plain careless.

 

 

Message 18 of 58
t_smith5
in reply to: t_smith5

Okay, I've attached my new file with the latest progress. I did copy a design from another Sketch and pasted it into the current one I'm working on. I've been trying to reduce the number of Sketches I have. It's another circle within a circle which is situated at the top. For some reason I can't get it constrained. I've tried the method in bunga's video with a smaller wheel. He was able to constrain one wheel to the Origin with a dimension and then the other with a different dimension. I tried the same thing with these additional circles and it just gives me the same dimensions for both. I've tried different methods but can't get them to be fully constrained. Unless I now need to constrain it the big one below...? That one I have managed to fully constrain now. ๐Ÿ™‚

 

I suspect I may need additional help with some of the still unconstrained parts, but we'll see.

Message 19 of 58
TheCADWhisperer
in reply to: t_smith5


@t_smith5 wrote:

1.  I've been trying to reduce the number of Sketches I have.

2. It's another circle within a circle which is situated at the top.


1. Actually that is the opposite of what most beginners should do.  For beginners a rule is often suggested one sketch/feature.  I have a general rule of usually no more than 7-10 entities in a sketch.

 

2. When something will not constrain - click and drag and observe the behavior.  This is the single most important tip in all of CAD.

 

3. I see a lot of duplication in your sketch.  In general, avoid duplication - there is a computational less expensive technique and it is easier on you too (get lazy - do less work).

 

2. 

TheCADWhisperer_0-1681076527019.png

When I click and drag your circles I notice that they do not stay aligned vertically with the Origin.

It appears to me that that is the Design Intent - so I simply add a Vertical Constraint between the Origin and the center of the circles.

Now when I run the click and drag tip again I see that the circles will only move vertical, but the vertical height from the Origin is not defined.  Simply add the vertical dimension from the Origin.

 

When in doubt - click and drag and observe.

Message 20 of 58
t_smith5
in reply to: TheCADWhisperer

Thanks for the advice. I may need to re-read it a few times to process some of it. ๐Ÿ˜…

 

But I have been getting into the habit now of deleting/fixing errors in the timeline. ๐Ÿ™‚ I'm also trying to optimise things and the number of Sketches made. Constraints are now the next thing. I'm also always checking for spelling mistakes in my forum posts etc.

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