Sketch planes making me insane

[fallenturtle]

I'm trying to sketch at an angle but running into issues where different sketch elements aren't on the same plane despite my efforts to make them so. I tried using the angled body surface to create a construction plane, but as you can see in the image some of the sketch is floating above it and since its at an angle its not a simple changing of the z position.

I want the sketch plane to be exactly on the surface of my body so that when I extrude downwards there isn't any shapes sticking out of the top.

How can I make sure my sketches are where I want them to be? Do I have to eye it?

[jhackney1972]

The file you attached will not open with the following message.  Please try and attach it again.  Normally what you need to do is create an Offset Plane from the angled face with a zero offset.  Need your model to verify.

[fallenturtle]

Sorry about that, I think this one might be better. Thank you for your time!

[TheCADWhisperer]

@fallenturtle 

Are you willing to start over from scratch with step-by-step instructions on how to do this correctly?

[jhackney1972]

Your sketch was not created on the sketch plane.  If you select your sketch and right click, you will see this in the context menu.  You will have to remove some dimensions to other features to allow it to move back.

[fallenturtle]

This is part of a much more complicated model so I don't think complete scratch would be feasible... Maybe just the lid part, but I'd still hate to have to redo the work I've already put into it and the way it lines up with the lower portion. Is this the only way address the issue?

[fallenturtle]

Thanks, I'll try that. Is it apparent how I did this wrong in the first place?

[TheCADWhisperer]

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@fallenturtle wrote:

 I'd still hate to have to redo the work I've already put into it....

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That is perfectly fine with me.  I can spend my time helping those who want to learn.

[fallenturtle]

Do I need to remove the constraints to make the option appear? I don't see it regardless if I select the shape or the lines individually:

[fallenturtle]

Ouch! I'm sorry! I didn't mean to come off as disrespectful... I do want to learn 😕

It's just that I've poured countless hours and filament into this:

So the idea of starting from scratch is very daunting.

Is it not possible to learn by just starting the sketch for this element of the project by scratch vs the whole thing?

Basically there's an screen that is being held to the lid portion via screws and nuts with the screws coming in through the top and the idea was to change this so that the screw attaches to the lid via the underside and screws into nuts that are pocketed, so to speak, into the lid. I was attempting to draw in a hexagon like shape so that the nut doesn't freely rotate... basically like this:

Except that's the version from the layer not being on the same plane as the body surface. I was going back and trying to redo the sketch for these properly but was having trouble getting things lined up right with the existing body because of the parallax effect I was getting between the body surface and the sketch.

Hope that makes sense. I do appreciate your time and didn't mean to come off as ungrateful. 

[TheCADWhisperer]

@fallenturtle 

A lot of techniques could be learned in a short time by starting over with step-by-step instructions.

[johnsonshiue · Accepted solution]

Hi! I took a quick look at this design. The first thing I notice is that some geometry on the "nut cubbies 1" Sketch seems to be on a different plane. I suspect the geometry was created with 3D Sketch option enabled. If the geometry should be on the same plane, I suggest you delete it and disable 3D Sketch option. Then recreate it.

Many thanks!

[fallenturtle]

Starting over for the full thing or just the lid that I initially showed in the OP? I am tempted by wanting to learn techniques as I'm sure I'm building models in ways that probably cause me more work then necessary.

[TheCADWhisperer]

@fallenturtle 

Start a new file.

Start a new sketch on the YZ Plane with the Origin position as shown.

Sketch and dimension the lines as shown.

Attach the new progress file here for next set of steps.

Click on the image above to enlarge the view. 

[fallenturtle]

I hope this is ok? I used a construction line to get the 20degree angle. 

Thanks!

[TheCADWhisperer]

@fallenturtle 

Using Construction Lines is fine - but you must fully define your sketches to have robust and predictable behavior as the model is edited.

Observation in CAD is a critical skill that must be developed.

[TheCADWhisperer]

@fallenturtle 

Once we have the sketch fully defined the next step is to Extrude - Symmetrically about the Origin plane a total distance of 105.

Then add a Fillet R4 to these 7 edges...

Click on image above to enlarge the view.

Now do a Shell feature selecting the two top faces to remove.

Set the Thickness to 1.5mm and then OK.

Attach the progress file here for next set of steps.

[TheCADWhisperer]

@fallenturtle 

Continuing on...

[TheCADWhisperer]

@fallenturtle 

...as we continue editing...

Observe that all sketches have red lock symbol indicating fully defined.

[TheCADWhisperer]

@fallenturtle