Fusion
I have tried both with entering a number and with the arrow .
I have narrowed it to some setting because if i do a new design ( just a box ) or use other design done before , some work and others dont
see new box , it deletes the surface as you change the value , done the exact same way
My guess here is that you have two overlapping bodies. Chamfer is working correctly on one body, but you are seeing the other body, which makes it look like the Chamfer is failing. There have been no changes to Chamfer in a long time.
Jeff Strater
Engineering Director
this link is asking for a login. You should be able to Export the file as a Fusion archive (F3D), and attach it here.
Jeff Strater
Engineering Director
yes, that is what I expected. Body1 and Body2 have overlapping geometry in the area of the chamfer. The chamfer has been correctly applied to Body1, but Body2 is occupying the same space, so you can't see the effect, unless you turn off Body2.
So, the question here is: why is there overlapping geometry, and did you intend that? Did you intend to chamfer Body1 or Body2? Did you intend to combine these bodies?
screencast:
https://knowledge.autodesk.com/community/screencast/9f441408-bbf6-4faf-84f3-d4072e5bba94
Jeff Strater
Engineering Director
Some good news, and some "opportunity for learning" here. The good news, is the design is easily fixable. When you did the combine of Body1 and Body2, you left the "keep tools" checkbox on:
This option says: don't delete the tools that were used to join the bodies together. So, Body1 is still there, which was probably not your intention. The fix is: edit that feature, uncheck this box, OK.
Now, that will cause the Chamfer to fail (remember, it was applied to Body1, which is no longer there). Again, though, just edit the Chamfer, and pick the edge on Body2 you want to chamfer. I forgot what the distance value was, so you will want to remember that before you make the first edit.
Here is a screencast showing this process: https://knowledge.autodesk.com/community/screencast/5d3b6db8-0d90-4608-8c9a-46de5bde099d
Now, the learning opportunity. I generally don't try to tell people how they should design. But, the method you use here (make standalone bodies, then use Move to position them) can be problematic in larger models. So, it is best to break the habit early. All those moves can get expensive, and are a bit less precise than you probably want. You can probably design this model much more simply using a different method of creating the geometry in place. Looking at a few introductory videos will probably help. I may try to design a part like this how I would do it, later today. There are hundreds of ways to do this, and yours is not invalid, but there are probably more efficient and accurate ways to do this.
Jeff Strater
Engineering Director
Here is a screencast showing one of the hundreds of other ways to create this shape. The pattern of: create a sketch, then solid geometry from that sketch is one that is widely used in CAD. The advantage is that the design is then fully parametric: You can later edit the sketch, change a dimension, and the design will adjust to the new size. If there is anything in here that is confusing to you, feel free to ask about it.
https://knowledge.autodesk.com/community/screencast/600407de-f037-45b4-bfc4-2742648f9159
Jeff Strater
Engineering Director
@freezing914 wrote:I would love to know more
i had all those parts made of welded and bent stainless steel, .
I am going to walk you through 2 different techniques.
STEP 1. Start a new file and make sure that Capture Design History is turned on.
(Check this by right clicking on the top node of the BROWSER.)
Once it is turned on it will say...
If it is already on - then you don't need to do anything (it was off in your previous file). The ONLY correct way to work is with Capture Design History turned on.
STEP 2. Start a new sketch on the XZ plane.
Sketch a rectangle above the Origin as shown...
(Be sure to dimension the Z height to 8 decimal places exactly as shown above.)
STEP 3. Add a Midpoint constraint between the Origin and the bottom horizontal line of the Rectangle.
What do you notice about the color of the Rectangle after this constraint is added?
STEP 4. Right click on the top horizontal line and select Construction...
(0r alternatively, left click on the line and mash the x key on your keyboard.)
File>Export the file to your local drive (not a drop box) and then Reply to this thread and Attach the *.f3d file here for the next set of steps.
The steps we are following are referred to the BORN Technique (Base Orphan Reference Node Technique if you wish to research.) This technique is predictable and robust. We will know exactly what is going to happen with any editing.
Extrude the three Normal lines of the rectangle using the Thin Extrude option as shown below...
Expand the Sketches folder.
Turn on the visibility of Sketch1 by mashing the eyeball glyph.
Right click on Sketch1 and select Dimension Visibility...
Double click on the 74.33150109 dimension and type in 70 and mash Enter.
What do you observe happening to the geometry?
Apparently in your original model you were "eyeballing" the sizes of your geometry. You can type in exact sizes and you can edit at any time and it will automatically update (that is what Capture Design History is all about).
