topic Betreff: chamfer working half way issue in Fusion Support Forum

chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 15:05:39 GMT

ok been learning the software and i am getting better but this morning i encountered a really odd issue .

so i have a series of boxes to create a shape . I used to be able to chamfer the corner easily using the right mouse click , etc . now the issue is that , it draws the line on the component as if it is working but if you click enter it does not complete it , it just draws the line on the component and does not remove the corner

I cant find any setting for it and worste of all , I did not change any setting , even went as far as doing a reset all setting but it still refuse to work

thanks for the help

Betreff: chamfer working half way issue

g-andresen — Fri, 02 Dec 2022 15:36:41 GMT

Hi,

Did you enter a size for the chamfer?

günther

Betreff: chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 16:08:32 GMT

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

Betreff: chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 16:17:37 GMT

I noticed that i was on the V8 version , the other that i have an issue is also at V7

is it because its the free trial version and it locks feature out as you go along ?

Betreff: chamfer working half way issue

g-andresen — Fri, 02 Dec 2022 17:04:14 GMT

Hi,

Please share the file.

File > export > save as f3d on local drive > attach it to the next post.

günther

Betreff: chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 17:52:14 GMT

here is the attached file , correction , it wont let me insert a file .

lets try this link

https://chromspec.sharepoint.com/:u:/s/int.instrumentation/EVsiNff4wcRBo-o2dfVyOiABgxBxW6inxd2jMzR5CbEK6Q?e=150h2y

I have made of the chamfer , that is incomplete on it

Betreff: chamfer working half way issue

jeff_strater — Fri, 02 Dec 2022 18:02:03 GMT

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.

Betreff: chamfer working half way issue

jeff_strater — Fri, 02 Dec 2022 18:03:23 GMT

this link is asking for a login. You should be able to Export the file as a Fusion archive (F3D), and attach it here.

Betreff: chamfer working half way issue

g-andresen — Fri, 02 Dec 2022 18:10:44 GMT

Hi,

share f3d this way:

File > export > save as f3d on local device > attach to next post

günther

Betreff: chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 19:00:39 GMT

found how to attach

here it is

Betreff: chamfer working half way issue

jeff_strater — Fri, 02 Dec 2022 19:28:44 GMT

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

Betreff: chamfer working half way issue

freezing914 — Fri, 02 Dec 2022 19:58:44 GMT

well , we are getting closer . I definitely messed up somewhere as i had no intentions to have body 1 and 2 overlap . and i have no idea how i did this , likely rookie error , can it be undone or fixed

I am still struggling with attaching 2 pieces and working on separate or combined pieces , must be related to the "combined" command . I also saw where i needed to add the half circle , i needed to combined the parts because the delete command did not work if they were not combined

I am trying to make simple bracket with a snap maker 3D printer and i see issue with parts that look attached in fusion that are not when printed , thats why i used the combined command

by the way , i could not unmute the video

is there a way to uncombine to fix this

Betreff: chamfer working half way issue

jeff_strater — Fri, 02 Dec 2022 21:39:20 GMT

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.

Betreff: chamfer working half way issue

jeff_strater — Fri, 02 Dec 2022 22:09:55 GMT

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

Betreff: chamfer working half way issue

freezing914 — Mon, 05 Dec 2022 13:10:05 GMT

thank you very much , this is very appreciated

I have saved the video of the sketching and will play with it , it does seem to simplify the process

Betreff: chamfer working half way issue

TheCADWhisperer — Mon, 05 Dec 2022 13:47:15 GMT

@freezing914

Are you interested in step-by-step instructions on how the pros would model this geometry?

Changing your techniques a bit would make all of this much easier and faster going forward.

Betreff: chamfer working half way issue

freezing914 — Mon, 05 Dec 2022 15:38:13 GMT

I would love to know more . watch a few videos, i went that way first because it was easier to visualize the 3D .

this morning i added the semi circle to the side and when i was trying to draw them , they seemed to " join to the face of the part and i could not move them , but if i turned the part 180 degrees , then i could

I am a chemist so all the CAD thing is really new . At home i can rebuild a car from scratch from stuff laying around the shop . made many paper drawings , its the learning . and i guess the learning the right way first is easier than learning the wrong way and have to forget about it once you are used to it . i had all those parts made of welded and bent stainless steel, originally made of a cardboard template, old fashioned you could say LOL

Betreff: chamfer working half way issue

TheCADWhisperer — Mon, 05 Dec 2022 22:08:22 GMT

@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.

Betreff: chamfer working half way issue

freezing914 — Thu, 08 Dec 2022 13:04:56 GMT

so far the instruction have worked

I am still playing with the new technique to redraw the same things for now

I have a new idea just need to find the time

Betreff: chamfer working half way issue

TheCADWhisperer — Thu, 08 Dec 2022 20:36:21 GMT

@freezing914

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).