Fusion 360 - How do I offset and offset line?

[Anonymous]

1. Start a sketch
2. Make a line
3. Offset the line
4. Now attempt to offset the line created in step 3

I can't get it to work. Can it be done?

[jeff_strater]

No, this is a current limitation of the new offset.  You cannot offset an offset curve.  Instead, go back to the original and offset it to the desired distance.

[Anonymous]

This is very silly, considering that workflow was very common in AutoCAD (my dad is a civil engineer, and would let me use his copies of AutoCAD, I used even DOS AutoCAD on a 286, and even then, many of my, and my dad sketches, started by making some lines, and offseting then, and offsetting the offsets like there is no tomorrow... For example to create grid-like patterns, or to create parallel lines, for example when drawing a "diagonal" room in a house... by drawing the first wall, and then offsetting the room size to create the other side, and then using snapping to draw the reaming 2 walls).

[TrippyLighting]

Your comparison to AutoCAD is rather silly 😉

You may simply have to get used to a different workflow when using Fusion 360.

The main purpose of the offset function in Fusion 360 os to offest a complet profile by a certain distance and do so parametrically, so you don;t have to manually elect every line, arc etc. offset it, constrain it properly and then dimension the offset. Altough, you can of course do that as well. While this newer parametric form of the offset tool can certainlty be improved and has limitaitons, it is very powerful for that purpose.

Offsetting a line from an already offset line is easy enough to do without the offset command:

1. Draw a line and constrain in it to something, if it is not already.
2. Draw a second line dimension the distance between the first and second line.
3. Draw a third line and dimension the distance between it and the second line.

[jeff_strater]

It's a fair criticism.  This is not a permanent limitation, it's on our list to address.  But (and I am biased here), the workaround does not seem terrible.

However, it is worth pointing out that Fusion offset is much more powerful than the AutoCAD offset tool, because of its associativity.  You can change the original and the offset will update accordingly.  You can change the offset distance, and the offset updates (including changes in the number of curves in the offset).  And, this is where the "offset of an offset" gets tricky.  If we start with this (the inner curve is the offset):

If you change the offset distance just a bit, we get:

So, you can see that the complexity of "offset of offset" can be a challenge:  New curves have been added that need to be tracked in the secondary offset.  So, we had a choice to make:  Either release it with this limitation, assuming that there is value in an intelligent offset, even with the limitation, or hold it back until we addressed this.  We chose the former.  I think it was a good choice, especially compared to the primitive offset that existed in Fusion prior to this change.

Jeff

[Anonymous]

You can do an offset of the offset line you have to release the offset constraint on the first to achieve the next. You may want to constrain it with a dimension instead

[cekuhnen]

@Anonymous @jeff_strater @TrippyLighting

you can also simply offset a new line with the expression

first line offset value + new value

this will make an offset that will look like an offset of the first offset.

https://drive.google.com/file/d/0Byzv_NlyKp_2RjZsbTRjdmFoWVk/view

[SaeedHamza]

Hi,

As @jeff_strater said, the best way to offset is by using the original sketch, other than that you'll have to delete the constrain every time you want to create an offset of the previous one

Here is a screencast to make things clearer

Regards

Saeed

[Anonymous]

Hello Jeff,

Is this feature of needing to only offset from the original wire entity going to change so we can offset an offset. The way it is doesn't feel user friendly and adds unneeded steps and time to drawing simple geometry. Is it possible to copy an entity multiple times?

[Anonymous]

Really would like this to work 😞

Especially when I change an offset profile now I have to do the chances twice.

[cekuhnen]

No you don’t have to do it twice - u only have to read my post above one time to understand that you can also reference the second offset distances to the first offset and then add the new value.

that allows you to do the same moving each offset independent yet affecting each other too

[Anonymous]

That's lovely.

It's also a cop out.

Let's imagine for a moment that I want to make a cylindrical case. It has in inner diameter D, and a thickness, X. Let's further imagine that it mates inside a lid part of thickness Y. Now, these are going to be real parts, so they need some nominal clearance, Z.

The parametric way to design this would be to draw that circle D, then create concentric rings offset by X, then Z, then Y units. In this simple example, drawing new circles is easy.

Once you want something at all more complex, offset *should* be the right tool. It sounds like this might be possible if you create offsets of X, X+Z, and X+Y+Z. This might be "eased" by referencing the earlier equations, but that's still a terrible workflow.

[chrisplyler]

Meh. I've not discovered a reason to care.

If I've got several concentric circles to sketch, I sketch one of them, and then offset the rest from it. In my mind, the two sets of concentric circles below are functionally the same, and the time delta between creating one set and creating the other set is 1.042892-seconds.

Now, doing the same thing with a more complex shape, made up of several lines, arcs, etc., would be more of a hassle to do as per the right-hand method above, because you'd have to re-dimension and re-constrain every element, causing more work and more clutter of dimensions and constraints. But since they're functionally the same in my mind, I'm just as happy to do it as per the left-hand method above.

So, yeah, I hope they improve the tool to do what is asked for in this thread, but I don't consider it a huge priority over things like FINISHING THE JOINT SYSTEM, DO YOU HEAR ME AUTODESK?!?!?!?

[TrippyLighting]

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@chrisplyler wrote:

... DO YOU HEAR ME AUTODESK?!?!?!?

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You spend a good bit of time here. How would you rate the participation of AD employees on this forum?

[TheCADWhisperer]

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@TrippyLighting wrote:

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How would you rate the participation of AD employees on this forum?

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I told Andrew face-to-face at AU a couple of years ago that the sketcher in Fusion is a mess.

Has it been fixed?

I realized a couple of weeks ago that I had become so accustomed to using workarounds that I didn't even think about it any more.  I would simply delete and try a different tact until I got something/anything to work.

https://autode.sk/33Nrf7r

[chrisplyler]

Considering that it is primarily a user forum...I rate their participation pretty highly. @jeff_strater  in particular is a beast of informative, professional helpfulness. A beast I say!

But my high rating is not meant to reflect upon their prioritization methodology or Chad's productivity rate.

[TrippyLighting]

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@chrisplyler wrote:

Considering that it is primarily a user forum...I rate their participation pretty highly. @jeff_strater  in particular is a beast of informative, professional helpfulness. A beast I say!

But my high rating is not meant to reflect upon their prioritization methodology or Chad's productivity rate.

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If no one but users responds, then that makes a user forum by default 😉

[Anonymous]

We agree, circles are straightforward. Once it's anything more complicated, that is a terrible defense.

Real world example: We have a PCB in an electronics box with a tongue and groove seal. That e-box is inside the enclosure that is the rest of our device. These enclosures are both to be injection molded. They are shapes other than circles or squares because 1) injection molded and 2) users have aesthetic preferences for shapes other than squares and circles.

At minimum, there are the following offsets to keep track of

• PCB to inside of e-box wall
• e-box wall thickness
• e-box inside wall to inside of groove
• inside of groove to inside of tongue
• tongue thickness
• outside of tongue to outside of groove
• outside of groove to outside of e-box wall
• outside of e-box wall to inside of product enclosure
• product enclosure thickness

There are many ways to skin this particular cat, but it seems the answer here is "learn to do it how we do; all other paths are either wrong or unimportant."

[chrisplyler]

No, the answer given by Autodesk here is, "We plan to get to it, but you'll have to work with what we've got so far until then."

Sure, for all practical purposes, those two answers have the same result for users right now. But the intent/attitude is quite different between them. One of them says, "Screw you guys, we don't care about you, deal with it," while the other says, "We know, you're right, we're trying to get to it."

And I don't think my defense was terrible. Okay, you've got fifteen offsets to keep track of. But still, it's just addition/subtraction to relate the total values to the individual values you would prefer. So you've got fifteen simple addition or subtraction problems to do. Or, as mentioned earlier, you can have them done for you by setting up your offset dimensions with formulas. So at worst, you've got to enter fourteen formulas or whatever. Personally, I consider that level of problem to be a minor nuisance...not a major catastrophe.

I've already agreed that it's a nuisance worth solving, I just don't think it's worth skipping lunch over.

[jeff_strater]

thanks, @chrisplyler - appreciate the kind words. 

I've posted variations of this many times over the years, but the basic problem we have is limited resources and nearly unlimited requests.  And, there is this very natural tendency to see each problem that exists as super important, because that is what you are currently experiencing at the moment.  Yes, I agree it is bad that you cannot offset an offset.  But, at the risk of putting down my own product, there are hundreds of quirks, bugs, deficiencies, etc. in Fusion.  Everyone sees their own issue as critical, and expresses outrage that it is not fixed.  I would love to fix the offset-of-an-offset issue.  I would love to fix the "can't use driven dimensions in an equation" issue.  I would love to add more joint types (we are looking at that one, @chrisplyler ).  @TheCADWhisperer beats us up daily about the sketch solver (though even he has to admit it has gotten better).  We have serious performance concerns.  Anyway, you get the idea.  We have to take this entire soup of outrage and figure out which few projects get the funding.  This one is on the list, certainly.  We will fix it someday, I just cannot promise when that will be.  In the meantime, there is a workaround, though I understand it is not great.