How Can I Combine Two Faces that Are Aligned on a Solid Body?

[Fab_Things]

I am trying to figure out how to eliminate the horizontal boundary line between the two highlighted faces.  This line went away on the sides when I got the faces aligned but, the highlighted one and the one on the opposite side still have this line.  I've tried zooming in to see if the faces are slightly off but when using 'measure' it never highlights a second line to select.  How can I combine two adjacent faces like the ones highlighted?  (design file attached)

[davebYYPCU]

Try Display > Visual Settings > Shaded, 

if the line disappears then you only have one face as selected in the pic.

Might help….

[Fab_Things]

I don't see a 'Display' option and when I search the help file, nothing comes up with 'visual settings'. How do I find this? I have the personal version of Fusion - maybe it's not available in that version?

[davebYYPCU]

Bottom menu, just right of centre, looks like a tv icon.

Might help….

[Fab_Things]

Thanks @davebYYPCU!  When I change that setting to what you suggested, the line does go away.  So, why would the line show when it's set to 'Shading with visible edges'? Why does Fusion opt to show two faces on one side but not on the two side ones? Is there some way to join those two faces so the design file looks cleaner?

[davebYYPCU]

If that and other lines do go away, keep that setting.

Visible edges are likely from the sketch endpoints.  Clean the sketch.

Might help….

[TheCADWhisperer]

@Fab_Things 

You are not using good modeling practices.

Would you like to learn how to do this correctly with step-by-step instructions?

You have a slight distance between those two faces.

Many other issues as well.

[TrippyLighting]

---

@davebYYPCU wrote:

Try Display > Visual Settings > Shaded, 

if the line disappears then you only have one face as selected in the pic.

Might help….

---

That is inaccurate!

You'll still have two faces, even if they are coplanar.

[TheCADWhisperer]

---

@TrippyLighting wrote:

---

You'll still have two faces, even if they are coplanar.

---

And in this case they are not even coplanar.

[g-andresen]

Hi,

Due to the "unfavorable" procedure, the surfaces were misaligned.
I eliminated this by removing surfaces and adding new fillets in a rustic problem elimination process.

günther

[TheCADWhisperer]

@Fab_Things 

I recommend that you do not follow @g-andresen video instructions.

Better to learn how to do it correctly from the start.

[Fab_Things]

Yes, absolutely @TheCADWhisperer!  I would greatly appreciate that!!  I want to learn the proper way to do this.  Thank you!

[Fab_Things]

Thank you @g-andresen for the video and corresponding updated file!  I will review the steps in the file 👍

[TheCADWhisperer · Accepted solution]

---

@Fab_Things wrote:

 I want to learn the proper way to do this. 

---

Before we get started - let's examine the existing geometry.

Notice that these two faces are also not co-planar.  A slight distance between the faces.

Same with these two faces on the other side - a slight distance... (are you familiar with Scientific Notation?  4.884E-06mm = 0.000004884mm)

and

5mm on this side...

and 4.993 on this side (click on images to enlarge the view)

This distance doesn't make logical sense?

These two faces are at a slight angle... (I assume design intent was for them to be parallel)...

Same on the other side - slight angle.

Give these issues found so far - the first question that comes to mind is, "Was it your Design Intent to have this rectangular hole offset?"  Is it your Design Intent to have the hole rectangular or square?

I suspect there will be a bunch of back and forth questions/responses required to flush out your true Design Intent for the geometry.

Also - many of your sketches are not fully defined (notice Lock glyph for fully defined sketches)...

[TheCADWhisperer · Accepted solution]

@Fab_Things 

Start a new part file.

Start a new sketch on the XY Plane.

Sketch a Center Point Rectangle at the Origin...

Notice that without dimensions the rectangle is blue...

Add the two dimensions and the sketch turns black indicating that it is fully defined and a Lock glyph appears in the browser on the sketch as another way to indicate that it is fully defined...

Now sketch a 2-Point Rectangle in space above the first rectangle...

Now add a Midpoint constraint between the top horizontal line of the first rectangle and the bottom horizontal line of the second rectangle...

Now add two dimensions to fully define the second rectangle...

I had to guess at the dimensions as yours did not make logical sense.

If your design intent is to dimension from the Origin to the outside edge rather than the 21mm, then do that instead.

Attach your progress *.f3d file here for next set of steps.

[Fab_Things]

Thank you @TheCADWhisperer!!!  I am working on this now! 👍

[Fab_Things]

Hi @TheCADWhisperer, thank you for taking the time to help me - I greatly, greatly appreciate it.

Answers to your post questions:
1. Was it your Design Intent to have this rectangular hole offset?
==>Yes
2, Is it your Design Intent to have the hole rectangular or square?
==>Rectangular

Overall Design Intent:
Create a bending die to use in a specific arbor press. The offset rectangle is dimensioned to create the proper bend and

allow the arbor press tool to pass through the opening based on the thickness of the metal being bent.

New .f3d file attached!

[TheCADWhisperer · Accepted solution]

@Fab_Things 

Delete those two construction lines - not needed...

White dots should keep you awake at night.

[TheCADWhisperer · Accepted solution]

@Fab_Things 

Now sketch another 2-Point Rectangle at the Origin (be careful not to click on the construction lines of the previous rectangle...

Add the two dimensions for the inside (hole) rectangle.

Now Extrude 

Make the Sketch visible again and Extrude the second rectangle...

[TheCADWhisperer · Accepted solution]

@Fab_Things 

Now right click on Sketch1 and select Edit Sketch

Add the vertical construction line from the Origin and the circle as shown.

Dimension the diameter and distance...

Finish sketch and then Extrude the circle in opposite direction...