Adding fillets de-references rectangle dimensions

[siriusphil]

I'm nearing the end of a complex (for me) design and needed to go back to an early rectangle sketch to add fillets.  When I do, the rectangle's location and size, which were dimensioned to the corners are now dimensioning nothing but each other.  Those two dimensions are referenced in many places later in the design so I get a warning when I try to delete them to recreate them referenced to existing points on the rectangle.  How do I re-reference the dimensions without losing the references?  

BeforeAfter

[g-andresen]

Hi,

please share the f3d file for investigation

günther

[siriusphil]

Here's the file.

[TrippyLighting]

No file was attached to your post!

[siriusphil]

I thought it was attached  last time.  Here it is again

[TrippyLighting]

If you are trying to attach a model to post using an email reply, that does not work.

You'll have to use the web interface.

In other words, there still is no attachment 😉

[g-andresen]

Hi,

try again

günther

[siriusphil]

You can see from the images I sent in my first post that the two dimensions on the right are referenced to the top right corner of the rectangle. Then I add the two fillets and the dimensions are no longer referencing the top of the rectangle because the corner has gone away. I just need to re-reference them to the point where the top of the rectangle is tangent to the fillet without deleting them and re-dimensioning, losing the references to those two dimensions later in the design.

[siriusphil]

I was using the web interface and the attachment is there on my end when I drag and drop it.

[TrippyLighting]

I don't usually put fillets in sketches if I can use 3D features to create fillets 😉 

[jeff_strater]

no, there is no way to re-reference a sketch dimension.  And yes, sketch fillet can be destructive to dimensions, as you observed, especially if you dimension to line endpoints. If you dimension to the line itself, instead, the dimension should survive.  Here is a simple example:

[HughesTooling · Accepted solution]

@siriusphil  I can't get this to fail but looking at the image in post #1 I think you have show points unchecked. If you enable it you should see points at the ends of the dimensions, you can then add a coincident constraint between the lines and the points. Just select the coincident constraint then click the line (not the end point) then click the point at the end of the dimension.

[siriusphil]

Thanks Mark, that works.

[Julie_7]

I was going to submit a feature request and then I saw this.

I think that when a rectangle is created, the dimensions entered should be set as the distance between the sides instead of the length of the side. This is still a properly dimensioned rectangle. However, it allows additional operations, such as corner fillets, to work without breaking/removing the rectangle dimensions.

[Julie_7]

Putting the fillet in the sketch has the benefit of being able to see the dimension later without having to edit the feature. I can just show dimensions on a sketch. As far as I know, there is no way to show dimensions on a 3D body, although I would find it useful.
I often have to resort to using the inspect tool or edit the feature to remind myself what the dimensions are.

[TrippyLighting]

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@Julie_7 wrote:
Putting the fillet in the sketch has the benefit of being able to see the dimension later without having to edit the feature. I can just show dimensions on a sketch. As far as I know, there is no way to show dimensions on a 3D body, although I would find it useful.
I often have to resort to using the inspect tool or edit the feature to remind myself what the dimensions are.

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Understood!

After over 30 years of professional CAD experience in Machine and Product design (20+ in Solid Works, 4+ in Alibre Design, 5+ in ZW3D, and almost 10 in Fusion 360. I won't mention AutoCAD ) I stand by what I said! Fillets and Chamfers do not belong into sketches, unless needed, e.g., for a sweep path.. 

[Julie_7]

I agree with you. It is better to add fillets and chamfers to the body.
If I think about it from a manual machining point of view, the body will get turned into a blueprint that will be used to machine each part. The blueprint will show all of the dimensions, both from the sketch and from the final body.
I have only been using CAD for a couple years, initially to produce blueprints for my personal machining work, and, but mostly for the last year to produce 3D printed objects. Because I no longer produce the blueprints, I often want to look at the CAD design to see the dimensions. I guess what I really would like it a way to "show dimensions" for a body that works similar to "show dimensions" for a sketch.

This is just my 2 cents, based on a novice and non-professional point of view.

[TrippyLighting]

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@Julie_7 wrote:
... I guess what I really would like it a way to "show dimensions" for a body that works similar to "show dimensions" for a sketch.

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That is possible in other CAD applications, just not yet in Fusion 360.