Three Queries No. 2. Rounding/trimming a corner

[Jaeger1787]

Good afternoon, folks.

I have created the valance at the bottom edge of the body shown in the picture. 

I need to trim these to length and fillet the corner edge - approximately 1mm radius.  I have tried creating the valance with a sweep feature, but this only lets me sweep along one edge.  I created (I think) an angled plane at a corner, hoping to use that as the base for a trimming tool to merge the two pieces of valance together, to no avail.

Any guidance on how to create a single valance along the face and two short arms is appreciated.  The file is attached.

Keith.

[demong · Accepted solution]

Hi @Jaeger1787 ,

I took a look at your CAD and took the liberty of adding the feature I think you want. I was able to make a sweep command work by choosing a different starting plane and holding the "Ctrl" key while clicking subsequent lines for the sweep Path. Take a look at the attached model and see if it gives you the result you're hoping for.

While you're in there, I would also recommend cleaning up and fully defining your sketches. You can see in the photo below that the valence you've mentioned does not meet up perfectly with the edge of the window/door-like feature.

That is because there is a very slight angle to the line in the sketch used to create the feature, which I assume is unintended. 

It may not matter for this model, but generally I would recommend making every line in your sketches fully defined before continuing. Sometimes spending a few extra minutes up front can save you a lot of troubleshooting later on.

I hope the attached CAD helps you. There are many different ways to achieve the feature that you want, so if you have any questions, ask away!

Best,

Jon

[Jaeger1787]

Thanks for your assistance, Jon. 

I thought that I had replied to your message a few days ago, but it seems that I failed to send the reply.  Essentially, I followed your advice and it worked perfectly for me.  I also took on board your comments re logging the sketches and using snaps.  I do try to do so, but sometimes Fusion seems to have its own ideas and I can not work out where I am going wrong.  Even something simple as dragging or extending a line gives me a headache when the entity becomes unco-operative.

Regards.

Keith.

PS.  All I need to do now is Accept the solution.  Now where has the button gone????

[TheCADWhisperer]

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@Jaeger1787 wrote:

I do try to do so, but sometimes Fusion seems to have its own ideas and I can not work out where I am going wrong. 

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@Jaeger1787 

You should immediately STOP and attach your file and ask questions whenever you cannot work out where you are going wrong.  Don't keep digging a deeper hole.

Your first sketch is missing the dimension of the baseline.

And when I add the missing dimension the current distance does not make logical sense.

[Jaeger1787]

Thanks for the encouragement to ask questions, although I sometimes feel I am being a pain in the neck.  May I say that I think this supportive forum is the absolute tops.  I am overwhelmed by the helpful responses and the number of topics raised.  It is obvious that some folks go above and beyond a quick answer and assist in solving my problem in a really helpful manner.  I suspect the answers to all my questions are probably already available, if one knew where or what to actually look for.  Many thanks guys.

[Jaeger1787]

In an earlier response, Jon said 'clean up and fully define your sketches......' which I do attempt to do.  However this is one of the problems I have found in attempting to do just that.  This picture shows the second of the two valances i am trying to create:

It is intended to be in the same plane as the door recess.  It appeared to snap to the bottom corner OK, but several other points would not do so.  I entered all the dimensions, but according to the line colours, it is still not fully defined.   What is missing?  What else do I need to do to a)get the lines to snap to a given endpoint, b) fully define the sketch.   Until I sort this, I can not sweep the valance around the edge. 

The working file is appended.  I observe that there appears to be an error with the sweep from the other valance, although on screen the feature appears correct.  Again, what is missing?

[TheCADWhisperer]

@Jaeger1787 
It appears that a Horizontal constraint is missing from the 3.5 line.

Why did you attach the stl file rather than f3d file?

[demong]

Hi @Jaeger1787 ,

I agree with @TheCADWhisperer , it appears that fusion isn't happy with the constraints. Without the .f3d, I can't open and inspect the CAD, but as a few guesses, try looking into the following:

In the sketch workspace, Fusion has a very nice "Project" tool, which I have navigated to in the below screenshot. (As an aside, I always use the hotkey 'P'.) If I am sketching to add a feature to existing geometry, I will begin by projecting (or intersecting, seen just below) that geometry to the sketch plane to give myself something to work off of. I believe Fusion will often try to guess objects that you need projected and do this automatically in some cases, but I find this less reliable than choosing the geometry myself and then hiding the bodies while I sketch.

The next thing I'd draw your attention to is the "CONSTAINTS" tab in the upper right of the screenshot, which @TheCADWhisperer hinted at. If you're unfamiliar, these give you a variety of ways to constrain your sketches without needing to dimension every line and angle. (I keep a variety of these as custom hotkeys for my commonly used constraints.) Again, based on how you sketch, Fusion will try to guess which constraints you want, but I often find myself deleting and replacing these. I apologize if this is stuff you already know, but I recommend getting very familiar and cozy with the constraints tab, as I find myself there constantly and it seems to improve my workflow. Here are some examples:

In this sketch, I used the projected vertical line and added 3 perpendicular constraints to the corners.

In this sketch, however, I still have the projected line, but I sketched over the construction line and added dimensions to all sides. The two left corners are held in place with Fusion's assumed coincident constraints (which is correct), but in order to fully constrain the sketch, I had to add two angle dimensions. This is more work, and I believe more confusing.

One troubleshooting technique I use often in my sketches is clicking and dragging sketch entities that may or may not be fully constrained. You can see in the below screenshot that the sketch has mistakenly turned black after adding the first angle dimension:

but if I click and drag the angled line, I can get this:

Then I know I can add the 90 deg angle (or better yet, the perpendicular constraint) to the upper left corner to get back to my intended geometry.

Hopefully that helps you troubleshoot the sketch and your CAD. Feel free to post if there are more issues.

[Jaeger1787]

Oops.  CAD file now attached.

Keith