I'm sorry if this is really trivial question but: how can I fill in the space between the walls of my model, so when I try to print it, it won't come out as just a blank space?
Fill in the space between walls
Sketch1 is missing many many dimensions and not making use of obvious symmetry about the Origin.
Sketch1 is also missing geometry constraints.
Start a new part file.
Create a sketch rectangle above the origin and dimension as shown...
Add a Midpoint constraint between the middle of the bottom horizontal line and the Origin.
What the color of the sketch.
What do you observe?
Sketch a second rectangle within the first rectangle and dimension as shown...
As with first sketch - add a Midpoint constraint between the bottom horizontal line of the second rectangle and the Origin.
What do you observe?
Add a third smaller rectangle within the second rectangle and dimension as shown...
Add an Equal (=) constraint between one of the horizontal lines of the third rectangle and one of the vertical lines of the rectangle.
Now add a Midpoint constraint between the right side vertical line of the third rectangle and the right side vertical line of the second rectangle.
What do you observe?
Now create a forth small rectangle and using only Equal (=) and Midpoint constraint make it equal to the third rectangle and placed symmetrically about the Origin.
Attach the file here for next set of steps.
@duris.samuel wrote:
the bottom line is now stuck to the center point even when i change the dimensions.
I don't see any dimensions in your image.
Already you are not following my explicit step-by-step instructions?
All of my instructions were to create a Rectangle.
Your second "rectangle" does not appear to be a Rectangle (did you not observe the difference between my image (color) and your screen)?
My instructions were to make the fourth rectangle Equal (=) to the third rectangle, not do add any dimension.
Oops, well this time I did forget about you...
Extrude all 4 rectangles a distance of 206
Turn the Visibility of the sketch back on
Extrude - Cut the area inside the remaining 3 rectangles as shown...
OK
Oops, I forgot a step - no trouble.
Drag the Timeline marker back before this second Extrude feature.
Hide Sketch1
Add a 5mm Fillet to the 8 edges shown (you can pick them right through the model...
Be careful to select Edges and not Faces.
Now drag the Timeline marker back to the end.
I see another mistake that I made that we will take care of in a few minutes.
Shell the part selecting the top face to remove...
Attach the file of your progress so far.
Next we learn the real power of history-based modeling as a time machine going back in time.
Keep in mind that I am not familiar with your geometry.
I made a mistake early on - but we will say that I did it on purpose to demonstrate how to edit a sketch. Yeah, that's the ticket to redemption...
Edit Sketch1 and select and Delete the two Midpoint constraints...
Click and drag the two small rectangles to the other side of the vertical lines...
Put the Midpoint constraints back in so that the rectangles are on the correct side.
Now Edit Extrude2 and CTRL (CMD on Mac) unselect the two small rectangle profiles.
Should be back to where we were...
Now drag the Timeline marker back to before the second Extrude (Fusion is a Time Machine from the movies).
Start a New Sketch on the top face...
Select the top face and mash P for Project.
Click OK
Finish Sketch and then select the Hole command...
In the HOLE dialog box make sure to select the Multiple Hole option
Set the bottom type and the depth that YOU want.
Drag the Timeline marker back to the end.
From the MODIFY drop down select Offset Face...
Select the four cylindrical faces shown and enter a distance of -.25
Attach your progress here.
Before we go further - can you explain the purpose of these holes?
If you are going to use for screw fasteners - exactly what are the specifications of the fasteners that you will use?
