Offset + filet + adjustment

[TomHa]

This maybe something I'm doing wrong, but if there is a video explaining it please share the link. I'm not a designer, I was using Fusion 360 and wanted to move to this product so I did

Fusion makes this a little easier for me to understand, so I hope it's just as easy in Alibre

Simple sketch,
1. 3 connected lines at 90degres. so they make a C
2. 20 mm base
3. 20 mm up
4. 10 mm across
5. add a 1 mm fillet at the 2 corners.
6. create a 2 mm offset in reverse

Now change the base to 25 mm and the sketch gets messed up.

Question:
Should not constraints be automatically added to the offset lines and fillet?
And it gets really messed up if you mirror it across the origin before you make the change.




I did the same steps in fusion an including the setup and results too.



Again the only change was the base from 20 to 25 mms

 

[gwbruce]

I recreated your sketch and was able to produce a mess up similar to yours although not exactly. I then assigned a tangent constraint to all of the fillets to the adjacent straight line (both the inside and outside fillets). You need to also dimension the offset in all directions. After doing this I was able to change any dimension and the shape would hold.



Hope this helps.

 

[NateLiquidGravity]

Alibre Design does not currently add constraints automatically when sketch entities are offset. It is an often requested feature.
If I understand what you are making - I would suggest sketching the outside or inside lines only then do a thin wall extrude and then mirror that.

 

[HaroldL]

@TomHa , Welcome to the forum. It looks like @gwbruce and @NateLiquidGravity have given you a solution to the immediate issue.

But if you need further training here is a link to the Alibre training page. You can select your level of Alibre there for additional training videos

Alibre Software Training Center

Alibre's Training Center has a variety of resources for our Alibre Design, Alibre Atom3D, and Alibre Workshop products. View our training center resources.

www.alibre.com

Also, there are a lot of training videos on the Alibre YouTube page.

https://www.youtube.com/@AlibreLLC

And if you have specific questions don't hesitate to post them here on the forum, someone is bound to help you out.

 

[TomHa]

thanks for the quick replies. I will try the suggestions. I was working on a 3d printed light hanger that was challenge to messure and it was trial and error. it was frustrating having to start over because of the issue. Reminded me of using Blender years ago.

I also found the Control Z undo does not work so I really had no option but to start over.

What I do not understand is why the constraints are needed at all on the offset. shouldn't the adjustment to step 2 be made then all the other steps just be applied with that change. (Sorry I'm a senior software developer)

Happy New Year

 

[HaroldL]

What I do not understand is why the constraints are needed at all on the offset. shouldn't the adjustment to step 2 be made then all the other steps just be applied with that change. (Sorry I'm a senior software developer)

Constraining the Offset sketch figures has been asked for and likely more than once.

 

[TomHa]

FYI: After I wrote my comment, I thought about a much better way to handle this whole thing. If I setup global parameter up front for the length of each leg, that will be the source of truth for all calculations to be built on as the screen is redraw. So I tried it. I defined leg1 as 20mm, leg2 as 20mm and leg 3 as 10 mm. Then I sketched out my drawing.
Change leg1 leg from 20 to 25 mm and That did not work.

Sorry, that is a bug. I have to assume that if I provide hard coded global parameters in the beginning, those parameters will be used for all calculations. As I change the parameters the drawing will be updated to match the new parameters.

Constraining the offset I do not think is the answer, re-calculating all the steps based on the changed/new data provided is a better way. Trust me, easier said than done, I get it

lenghtOfX = 20
offset = 1
endPointX = lenghtOfX + offset
endPointX = 21

Change lenghtOfX to 25
endPointX = 26

Again sorry 30+ years of software development including 3d rendering systems, makes me put on my analytical cap on way to much.

 

[idslk]

Hello Tom,

are you using Version Atom, Professional or Expert?

Regards
Stefan

 

[NateLiquidGravity]

It is not a bug. It just simply draws in the offset lines/arcs at the offset you specify. It does NOT define a relationship between the original lines/arcs and the new lines/arcs. Should it? YES
Trying to change the original size by any method will still change the same thing and result in the same mess.

 

[stepalibre]

Is this the desired result?



If yes, the order is roughly:
- Fully constraint the inner or outer profile
- Offset it (don't touch it)
- Draw reference lines between the inner to outer points
- Make those reference lines equal
- Make the arcs concentric tangent
- Make the offset lines vertically and horizontally constrained
- Dimension the line representing the thickness.
Some steps can be done in any order.

 

[idslk]

create a sketch like Nate said:



create a thin extrude:



add fillets:

 

[JimCad]

Works fine with the "reference" lines to keep the arcs constrained.
Jim

 

[Ex Machina]

By the way, this could be perhaps done better with a thin-extrude.

But yeah, an offset constraint needs to become a thing. Although you should be warned that it frequently fails in Fusion, especially when the offset is changed so that a fillet disappears or becomes a point.

 

[idslk]

By the way, this could be perhaps done better with a thin-extrude.

like in post #11?

 

[NateLiquidGravity]

like in post #11?

Or post #3?

 

[stepalibre]

As a structural designer I want a full profile/cross-section sketch so all my calculations are defined inside a single feature.
As a CAD designer I'll use the thin-extrude approach.

* The thin-extrude + fillet features approach can add extra overhead when building assemblies and making changes. When you change the sketch, all the features need to regen/recompute. If you have many instances, that will start to add up. If you add cuts, chamfers, fasteners, welds, and so on..

With simple parts the difference in overhead and performance is likely negligible.