Bodies extruded perpendicular have one face at an angle

[Anonymous]

I've searched quite a bit but it's difficult to find a search term. I created two bodies from separate sketches which are perpendicular. most of the faces are perpendicular as expected but if I inspect two faces on one side it shows a very small angle between them. I've tried deleting the feature and re-doing it and I've completely re-created the second sketch but I can't find where the discrepancy is coming from and its always in the same place.

The first picture shows the weird angle, the second is as expected and all the other three sides show the expected 90 degrees and the bodies themselves all measure as expected.

I appreciate the error is tiny but I think it's causing problems later as I add to the complexity of the design and start getting weird issues where extrusions don't match up properly or lofts refuse to recognise the face is in the correct plane.

I'm guessing its a rounding error related to the view because the measured angle changes if I rotate the model (third picture) but if someone can spot a schoolboy error I would be grateful

[davebYYPCU]

Can see what's there, but can't see how its made.  Can the file be shared?

There was a similar thread like this, with Extrude to Object, (Symmetric) if you have used this, it's somewhere to focus the effort.

[Anonymous]

Thanks for the feedback, it was created by extruding from one sketch then drawing another on a face perpendicular to the original sketch and extruding that, it doesn't matter if I join or create a new body those particular faces (right hand side of assembly, body1 of Duct:1 and body 3 of the parent component always display the issue even though both of show no such discrepancy when measured against the 'faninsert' component. 

Happy to share the file but when I attach it to the post it won't allow me to proceed - rendering the above meaningless 🙂

[HughesTooling]

Did you export as an f3d and reply using the forum, not by email? Other option is to ZIP the file then attach. One last thought on why you can't attach the file is, I think there's a size limit.

Mark

[Anonymous]

ok, realised I'd left an embedded component in there, breaking  the link leaves some errors in the later part of the timeline but the problem is in the first 2 sketches/3 extrusions

Playing around with it convinces me its an interface error rather than anything else, if I zoom in very close I can make the discrepancy disappear

[TheCADWhisperer]

Well, there are too many issues here for me to take the time to resolve each one, but starting with your first sketch - the very foundation of your design:

It is way too complicated and has dimensions that do not make logical sense from a Design for Manufacturability/Inspection/Assembly standpoint.

Dimensions should only go to logical datums.

Most fillets should usually be done as Features rather than in sketch.

Shell feature would eliminate many sketch elements/dimensions.

Do you really really intend inside and outside arc the same radius (see red circle).  This results in non-uniform wall thickness that is generally avoided in design.

The more I look at just the dimensions in the image below - the more I think - start over.

Practice creating simple, easy to decipher sketches and stop and post here at the first sign that things are getting complicated.

[HughesTooling · Accepted solution]

I second what @TheCADWhisperer says about the sketch being far too complicated. Better to draw the outside shape without the fillets, extrude, shell then fillet the solid body.

I found the problem with the out of perpendicular face all comes back to the sketch and one corner is not square, I guess the sketch solver is just pushed past it's limits trying to solve all you've thrown at it.

Here's a screencast that shows the problem corner. I guess the solver should be flagging the sketch as over constrained but with so many dimensions and constraints even then you'd find it hard to know where.

Mark

[HughesTooling]

And one more tip, take a look at the Rule #1 thread.

Mark

[TheCADWhisperer]

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@HughesTooling wrote:

... Better to draw the outside shape without the fillets, extrude, shell then fillet the solid body.

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I think I would probably Fillet, then Shell the body.

[Anonymous]

Thanks, appreciate you all taking a look and... I knew you'd say that 🙂 In defence of where it stands now the vast majority of those dimensions were added after I discovered the issue because I thought fully constraining the sketch might fix it, about half way through I knew it was getting way over complicated for what it is but I wanted to chase down the cause of the problem and if I submitted a largely 'blue' sketch I knew I would be told to constrain it better.

However I hit a problem because the simple version was a few circles joined by lines and arcs and then two offsets of the compounded curve,  every 'proper' dimension created an 'over-constrained' error so I had to remove the offset 'constraint' and dimension each element individually. I've learnt since to constrain the base curve before doing the offset; I picked up the 'filleting within sketch' from one of the instructional videos but will avoid it in future.

In the case of the highlighted item I can see your point but if I remove the radius the arc turns blue so I need to figure out when the general advice 'all sketches should be fully constrained' turns into 'you have too many dimensions' - presumably there's a happy medium which correct dimensioning will drive me towards but, as I said, the complexity in the sketch was driven by the discovery of the error not the other way round.

[Anonymous]

Thanks the screencast is awesome and points directly to the original mistake, just one further question - if I have 3d sketch disabled and the line has a horizontal/vertical constraint then do you have any idea how I managed to create that line at an angle to YZ?

[HughesTooling]

I've seen problems like that before and I just think it's down to overloading the solver. Once the error's there it seems like you have to delete the line, only seen it in other peoples sketch like this with way too much going on. Did you use an offset at some point then trim?

Mark

[HughesTooling]

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@TheCADWhisperer wrote:

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@HughesTooling wrote:

... Better to draw the outside shape without the fillets, extrude, shell then fillet the solid body.

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I think I would probably Fillet, then Shell the body.

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I assumed he wanted the 1mm rad inside and out as he'd gone to the trouble of dimensioning them like he had but yes if he wants a constant wall then fillet first.

Mark

[Anonymous]

yes I totally used offset then trimmed - this is a known bad practice?

[Anonymous]

hmm, spoke too soon, the angle is gone but now there is an infinitesimal gap between the extruded bodies, I guess I'll start again and try to tidy it all up

[HughesTooling]

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@Anonymous wrote:

yes I totally used offset then trimmed - this is a known bad practice?

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Not necessary but Fusion will add constraints when you trim and it's hard to track what's going on, OK with a few lines but not in a sketch like yours. In the screencast I made I'm not sure what's keeping the bottom line horizontal after I delete the parallel constraint for example, think it one of the many 1.32 dimensions. Honestly looking at the sketch is painful, maybe the sketch solver should show over constrained but you really don't need sketches this complicated.

Mark

[Anonymous]

Yes the sketch is now a mess, but as I said before the silly number of constraints was added in an attempt to solve the problem, they weren't the cause of it. I've changed the way I use offset and will be aiming for a less is more approach to constraints but Sketch is inconsistent and lacks transparency around its errors and warnings, it seems like it has foibles that have to be learnt like a book of ancient lore.

[pavel.kryda]

I have a similar problem in every project. This is one example of many.

The command extrude causes non perpendicular face.

I can´t measure distance on this face, because there is randomly generated angle.

This behavior is wrong because the errors add up.

In some cases it is not possible to make a joint.

Geometry built on this face does not fit with others.

Please see:

https://autode.sk/31kCaDO

What am I doing wrong?

[HughesTooling]

This comes down to your first sketch is not constrained and the use of sketches off faces off other sketches and model is just accumulating errors. Just fully constrain the fist sketch and it work as expected.

Mark

[pavel.kryda]

You saved many hours of my life. Thank you for the amazing support.