topic Re: Can't create a flat pattern in Fusion Design, Validate & Document Forum

Can't create a flat pattern

dmac252a — Sun, 17 Jul 2022 10:38:25 GMT

could use some guidance, I am trying to model a dreadnought guitar side cutting pattern. I've created a sheet metal component and modeled the one side with necessary back radius and appropriate top neck angle trimmed for my model. I am attempting to create a flat pattern from the component however I cannot select a stationary side. i have attached the file I'm working with. Advice and or modeling correction would be greatly appreciated.

thanks

Re: Can't create a flat pattern

aliobidi — Sun, 17 Jul 2022 11:01:14 GMT

Hi,

there is a lot of warning (yellow icons )
you should remove it
also where is the first sketch ?

Re: Can't create a flat pattern

TrippyLighting — Sun, 17 Jul 2022 12:42:09 GMT

1. You cannot select a stationary side, because that needs so be a straight section. It can be very short , but it has to be straight.

2. Looking at the timeline in general, I would re-design this from scratch. You deleted the 1st sketch, which is a complete no-no in a timeline based design. Using a position capture feature in such a design is completely unnecessary.

Have you completed any of the beginner courses accessible directly through the question mark in the upper right corner of Fusion 360?

Re: Can't create a flat pattern

dmac252a — Sun, 17 Jul 2022 13:06:29 GMT

1. Ok I will go back and start it again.

just as a fYI, my work flow seems pretty simple from a amateur’s perspective. I imported a DXF And validated the scale. Then created a flange the height I needed, created some drawings that trimmed the angle and radius of each end. Then attempted to do the flat pattern.
2. Was not aware of feature using the ? Definitely going to check that out.

thanks, will see how it goes

Re: Can't create a flat pattern

dmac252a — Sun, 17 Jul 2022 13:56:40 GMT

Here is a second attempt at the part. not really sure I understand where the straight stationary side has to be. I trimmed the front and rear edged square. the original DXF edges were slight angles..

Re: Can't create a flat pattern

jhackney1972 — Sun, 17 Jul 2022 13:59:21 GMT

I used your original file to create a new one in order to keep the general shape. I explain my process in the Screencast. This model does not have any of the width cuts you had in the original, I just wanted to give your a better start. Try to keep your timeline clean as you go along. Model is attached.

Re: Can't create a flat pattern

dmac252a — Sun, 17 Jul 2022 16:30:32 GMT

Selecting works fine when I use your file but when I create a new one I still cannot select a surface. The first thing I noticed was that you component (sheet metal) icon is at the top level whenever I create a new component it is at a sub-level.. I don't know if that is significant. I have created a new file. then created a new sheet metal component. I brought in the outline. first I extruded to the height ( I also tried to flange ) I added a .25" new body ( I also tried adding with the join) to the edge as you did. Still unable to select any surface to unfold or create flat pattern I looked pretty straight forward watching you do it.

Dennis

Re: Can't create a flat pattern

TrippyLighting — Sun, 17 Jul 2022 16:49:35 GMT

Ok, while that does look better in that it does not contain any yellow waring icons in the timeline, lets take this back right to the first sketch.

Generally, a large number of problems are reported from uses who import DXF and SWG files, mostly because they have no idea what it is they are actually importing. The first thing I do is to inspect the curves in the imported sketches with the curvature comb tool. Right-click on a curve to select t, then left-click and select :

This is the curvature comb of the outer curve. Smooth!

This is the curvature comb of the inside curve. Not absolutely terrible, but not as smooth as the original!

So for this exercise we're going to use the outside curve.

I've changed those sketch objects we're not going to need into construction lines/curves and then used the fix constraint to lock them into place.

Then I added a short straight line tangential to the front of the outside curve:

That is the straight segment I was referring to earlier.

Now you need to sheet up a sheet metal rule with the thickness of your material.

As we create a flange toward the inside, we'll set the K-factor to 0. That will result in the long edge of the unfolded sheet metal object being the same length as the curve then flange was created from.

I used .5" as the material thickness to make more visible what I did. YOU can change the material thickness to your liking.

Now you can continue with your design.

Make sure all your sketches are full defined, meaning they are fully dimensioned and fully constrained!