Hello,
I am trying to split this tube with the bowl so I can remove everything under the bowl (highlighted in the picture), but whenever I do, I get "the operation failed, try adjusting the values or changing the input geometry" I have also attached the .f3z file. Please help.
Why are you using an external reference?
Are all of your sketches fully defined?
Edit: Are any of your sketches fully defined?
Are you willing to start over from scratch with step by step instructions?
If I start to add missing dimensions - they do not make logical sense?
If this were my design I would have had a much more simple sketch and used a Shell feature instead.
Is something like the Attached what you are after (not the way I would really do it - but trying to narrow down your true Design Intent. I assume you want some holes going through too.)
Step 1. Start a new file. Start a new sketch on the XZ Plane.
Sketch a vertical line from the Origin a length of 2.176 as shown below...
Right click on the line and select Centerline.
Now sketch a Horizontal line from the Origin to the right and a Vertical line from the end of the horizontal line...
Dimension as shown. The Ø6.00 diametral dimension is achieved by selecting the centerline.
Sketch a 3-Point Arc and dimension as shown (I had to guess the actual dimension as your sketch didn't make logical sense for this radius).
Now Revolve the sketch about the centerline.
Add a R 0.2 Fillet to the edge as shown below (it is almost always better to add Fillets as placed features on the solid body rather than in sketch. I had to guess on the Fillet radius as your model didn't make logical sense.
Turn the part over and run the Shell command selecting the bottom face to remove.
Enter the desired thickness.
Q1. Will this design only be 3D printed, or will it be fabricated from metal components welded/soldered together?
Q2. If fabricated from multiple metal components - will the attached components protrude through holes in this component or will they be flush mounted to the outside face (the pipe nozzles, not the hex fasteners - we will get to those).
Attach your progress *.3df file here for next set of steps.
Right click and Edit Sketch1.
Sketch the angled 3-Point Rectangle approximately as shown below...
Add a Coincident Constraint between the corner of the Rectangle and the Centerline as shown (be sure to select the Centerline and not the midpoint of the centerline or the endpoint of the centerline).
Now dimension the angle as shown below.
Add the remaining dimensions as shown below...
Finish Sketch and then Revolve - Cut...
Mirror the Feature about the YZ Plane...
Attach your progress file here for next set of steps.
OK, let's continue.
Edit Sketch1
Add these three lines as shown below...
Now add a Coincident Constraint between this point and the horizontal line (I just realized that we made a mistake with the Ø4.6 dimension - but we can take care of that later).
Now add the Ø0.552 and the 1.825 dimensions as shown below...
Note that the sketch turns black indicating that it is fully defined.
Finish Sketch.
Drag the Timeline Marker to just after the Shell feature and before the Revolve-Cut.
Now Revolve-Cut the smaller hole as shown below...
Select Move/Copy and then the Rotate option...
Set to Move Object - Faces
Set the Axis as the Z Axis...
Enter 60 as the angle and select OK.
Drag the Timeline Marker back to the end of the Timeline.
Now start the Mirror command and set to Object Type > Faces.
Select the face of the small hole as the object to mirror and the XZ Plane as the Mirror Plane...
Run the Mirror command again, this time selecting both small hole faces and the YZ Plane as the mirror plane.
Attach your progress file here for next set of steps.
Fusion
