In this lesson, we will look at an editing workflow we touched on on a previous lesson,
that is often overlooked,
but can be incredibly valuable when it comes to working with data from other CAD systems,
as well as being a quick way to make changes to your designs.
First, let's go to the Tier 1 folder and upload the direct edit file.
When the upload is complete,
go ahead and open it,
in Fusion 360 and hide the data panel.
Looking at the component,
it's a simple plate with four holes.
But make note that the holes, on the nearest end,
are not concentric with the fillets on the part.
The part was created in Fusion 360 and the features are in the timeline below.
Sketches for the main body and holes and affiliate feature, or the corners.
Now let's turn off design history using the gear icon in the lower right.
Direct editing can be a powerful tool for developing shapes
quickly and for editing models that don't have a feature history.
Or if you need to make a quick change and don't want to sort through the design history.
In fact, direct modeling tools can be used with history on,
and the edits will be recorded in the timeline.
Well, now let's make a few changes to the play,
starting with the diameter of the holes.
We'll start the press pool tool and select the faces of the four holes.
You'll notice that when you select the faces,
an offset faces dialog appears.
Depending on the geometry you select,
press pool will give you different tools,
that are appropriate for your selection.
The mini dialog shows that the holes are five millimeters in diameter.
You can drag the new value,
or will simply enter 7.5 and press enter,
to change the size of the holes.
The whole diameter will be updated,
but they will remain centered where they were located.
Next we will move the two holes,
to be concentric with the Fielitz.
Start to move copy to or from the modified menu and switch the move object type to face.
Now select the faces of the two holes.
We can use either the free move type,
or the translate type.
For free move, we'll need to establish a pivot point.
Select the icon in the dialog,
then pin the center, to one of the holes.
Once the pivot is set,
be sure to select the checkmark,
so that Fusion 360,
knows you're done changing the pivot point.
Now you can pull the arrow,
aligned with the x axis and start dragging the location.
You can see incremental move is switched on,
or you can enter the distance value.
We can also change the move type, to point to point.
For the move you want to make, this should work well.
After switching the move type,
pick the center of the hole and then,
the center of the fillet and click OK to save the change.
Now we need to make a change to the overall size of the plate.
We can use press pull or move copy for this operation.
Though there are times where you might find one works better than the other,
depending on the geometry you are selecting.
For this lesson, I'll use the move copy tool.
Once it's open, I want to make sure that objects is still set to faces,
select the two fillets and the end face of the plate and the two holes.
Then, switch to the translate option and use
the arrow to move the objects 35 millimeters.
At any time you can turn design history tracking back on.
We can see the original sketches remain,
but the features based on them,
are no longer associated with the sketches.
Since this is a single standalone part,
that was just created as a body at the top level rather than building a component,
or the edits that this part might need,
we could just simply use direct modeling tools.
To thicken the part,
we can just use press pool and add another five millimeters.
When we are finished, we can save the file and move on.