Seeing edges after fusion

[AliHatukai]

Sorry if im a pain but im still a newbie and cant figure this out,
I have this designed mold i wanted and i have done everything and all and its done from my point of view,
But it bothers me that when i did the fusion action (several times) i still see edges between the shapes.
In other stuff i did with this program the edges would disappear.. what did i do wrong here ?

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13541 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 9948ee4f1570df9216862a79705afb367b2c6ffb
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: Hebrew/Israel (he_IL)


Thanks in advance.

[NormandC]

Version: 0.17.13541 (Git)

Version 0.18 has been out, please do yourself a favour and upgrade. Download

But it bothers me that when i did the fusion action (several times) i still see edges between the shapes.

Your original sketches are not fully constrained. There must be some very minor tolerance issue that causes faces not to be co-planar, so the Refine property under the Fusions cannot fuse the faces together.

Sketch under Body/Pad001 has multiple errors:

• The upper horizontal line to the right has a block constraint. Why did you use this? The block constraint was added to constrain B-splines because they can be quite a pain to fully constrain, for simple elements like lines you should never use the block constraint, but constrain them properly.
• On the same line, you added a point on object constraint to the arc, when it should be a point on point (coincident) constraint linking the two vertices.
• You should constrain the length of the lower longer horizontal line that lies on the sketch axis. Doing so after deleting the block constraint gives a value of 68.0015 mm. Was that intended? Shouldn't it be 68.0 exact?
• The vertical line to the right is not connected to the bottom horizontal line. It needs a coincident constraint.
• On the vertical sketch axis, there are two superimposed vertical lines. If you make a box selection over the sketch origin point then hit DEL to delete any coincident constrain, you can then move the elements away and reveal the duplicate line. Another way to prove this is to look at the Elements list at the bottom of the Tasks tab: it lists 7 elements, when obviously there should be 6.

That being said, why did you create two separate bodies? In my opinion, this should be much simpler to manage in a single Body; it should also be possible to use PartDesign MultiTransform containing 2 PartDesign Mirrored features to create the whole shape without having to use Part Mirror and Part Union.

[NormandC]

Have a look how this model can be much simplified by changing your thinking: rather than only thinking of fusing building blocks together, start with the idea that you are working from a block from which you will remove material, as in the machining process; or as a sculptor.

1. Start with a sketch that combines elements of both your original sketches to create the outer contour of your final model.

   

   FC_AliHatukai_Mold_01.png (27.65 KiB) Viewed 488 times

2. Pad this sketch to the full height of the final model, 25 mm.

   

   FC_AliHatukai_Mold_02.png (3.46 KiB) Viewed 488 times

3. Now select Pad, then press the PartDesign MultiTransform icon. In the MultiTransform parameters in the Tasks tab, right-click in the bottom white field and select "Add mirrored feature". Leave the mirror plane as "Vertical sketch axis" and press the bottom OK button.
4. Add a second mirrored feature, this time change the mirror plane to the horizontal sketch axis and press the bottom OK button.
5. Complete the MultiTransform by pressing the upper OK button. If the Refine property is set to true, you will see that all residual edges are removed:

   

   FC_AliHatukai_Mold_03.png (6.04 KiB) Viewed 488 times

6. Create a datum plane attached to the XY_Plane and with an attachment offset of 10 mm in the Z axis.
7. Create a sketch on the datum plane, and sketch a rectangle; hide the MultiTransform and show the first Sketch, then use external geometry to pick a point on the sketch. This linked external geometry from sketch will be more robust than a point picked on the MutliTransform feature. Use this linked point to add a point on object constraint with an horizontal line of the rectangle. EDIT: I made a mistake here, the rectangle should be wider so there is no need to use external geometry here; a simple vertical distance constraint on one side of the rectangle will do.
8. Complete the constraining with a symmetric constraint between two diagonally opposed points and the sketch origin point; then add a horizontal distance constraint to define the width of the rectangle.

   

   FC_AliHatukai_Mold_04.png (15.5 KiB) Viewed 488 times

9. Exit the sketch and create a PartDesign Pocket; check "Reversed" and set it through all, and press OK. You're done, and with a single Body!

   

   FC_AliHatukai_Mold_05.png (6.75 KiB) Viewed 488 times

[meme2704]

hi
if I can afford my comment:
Do not make 2 bodies, Sketch 001 must be linked to the Pad base by using the referencing ridge tools (blue) pad that makes the rims designated purple, this allows to have perfectly aligned ridge and similarly length
then at each miror fuse and refine = true

[AliHatukai]

Have a look how this model can be much simplified by changing your thinking: rather than only thinking of fusing building blocks together, start with the idea that you are working from a block from which you will remove material, as in the machining process; or as a sculptor.

1. Start with a sketch that combines elements of both your original sketches to create the outer contour of your final model.
   FC_AliHatukai_Mold_01.png
2. Pad this sketch to the full height of the final model, 25 mm.
   FC_AliHatukai_Mold_02.png
3. Now select Pad, then press the PartDesign MultiTransform icon. In the MultiTransform parameters in the Tasks tab, right-click in the bottom white field and select "Add mirrored feature". Leave the mirror plane as "Vertical sketch axis" and press the bottom OK button.
4. Add a second mirrored feature, this time change the mirror plane to the horizontal sketch axis and press the bottom OK button.
5. Complete the MultiTransform by pressing the upper OK button. If the Refine property is set to true, you will see that all residual edges are removed:
   FC_AliHatukai_Mold_03.png
6. Create a datum plane attached to the XY_Plane and with an attachment offset of 10 mm in the Z axis.
7. Create a sketch on the datum plane, and sketch a rectangle; hide the MultiTransform and show the first Sketch, then use external geometry to pick a point on the sketch. This linked external geometry from sketch will be more robust than a point picked on the MutliTransform feature. Use this linked point to add a point on object constraint with an horizontal line of the rectangle. EDIT: I made a mistake here, the rectangle should be wider so there is no need to use external geometry here; a simple vertical distance constraint on one side of the rectangle will do.
8. Complete the constraining with a symmetric constraint between two diagonally opposed points and the sketch origin point; then add a horizontal distance constraint to define the width of the rectangle.
   FC_AliHatukai_Mold_04.png
9. Exit the sketch and create a PartDesign Pocket; check "Reversed" and set it through all, and press OK. You're done, and with a single Body!
   FC_AliHatukai_Mold_05.png

I must say I didn't expect someone put this much effort in helping me, This is amazing, Thanks a lot!!
It is much more simple this way.

hi
if I can afford my comment:
Do not make 2 bodies, Sketch 001 must be linked to the Pad base by using the referencing ridge tools (blue) pad that makes the rims designated purple, this allows to have perfectly aligned ridge and similarly length
then at each miror fuse and refine = true

You can afford your comment and it is much appreciated. Thanks!