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Sheet metal practice

tyc

Member
Hi everyone,

How can I draw the attached part using only sheet metal environment in Alibre?

It is way faster not using sheet metal, because I cannot do circular pattern for a body created by sheet metal commands. If I could make a circular pattern of the first "Contour Flange" feature, it would be a lot easier to draw the part. If I don't use sheet metal environment and I need to have the flat pattern, then I have to use Convert to Sheet Metal command which creates one more file for the same part.

My Alibre file (Sheet metal) --> 21-02-11 LIGHT MOUNT(1).AD_SMP
My Alibre file (Solid) --> 21-02-11 LIGHT MOUNT SOLID PART.AD_PRT

What do you think? is there any other way you could come up with?
Thanks.

Shout out to TooTallToby for the drawing.
 

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    vgaBTNR.png
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  • 21-02-11 LIGHT MOUNT SOLID PART.AD_PRT
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GIOV

Alibre Super User
In ADV21 I did the part using the Sheet Metal WorkSpace. You are right is not feasible to do a Feature Circular bend Pattern
The weight is 815 Gm in Flat Carbon Steel 3 mm Thickness.
1674676813298.png

1674677741547.png

The vertical high is 60.091 mm, so is little more the total of 60 mm.
 

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HaroldL

Alibre Super User
@tyc , that is an interesting part and although it is a simple one it can be a challenge. It seems the more sheet metal tools Alibre adds the more options that are available for creating sheet metal parts.
I recorded a "short" video of a work flow using the Sketched Bend tool that you may find interesting. Here is a screen shot of the a drawing of the final dimensions using my method.
Practice Part for Ty.jpg
As you can see there is a slight discrepancy with the length of the bottom tab when measuring to the virtual sharp. I'm not sure how to resolve that issue using the method shown in the video.

https://www.screencast.com/t/ayUQXJY3
 
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OTE_TheMissile

Alibre Super User
If I had to model this, I'd designate the top "arm" as the master and drive all the other 3 arms' features through the Equation Editor. Then adjust the length of the inside flanges to get the 60mm height (through some napkin-scribble trig) before tuning the length of the outside flanges to get the 300mm BCø
 
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HaroldL

Alibre Super User
@tyc,
I think in the video I stated that I didn't know how to control the two dimensions on the bottom tab of the legs. After giving some thought to how I created the model it dawned on me that the position of the first sketch bend controls the location of the second sketched bend and affects both the 60 mm to virtual sharp and the 56.5 mm to start of bend dimensions.

So after some tweaking I get this:
Update for Practice Part for Ty.jpg

And just in case you have v26 here is the model for analysis. If you are on a previous version then hopefully the video will guide you through the workflow.
 

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tyc

Member
@GIOV
In ADV21 I did the part using the Sheet Metal WorkSpace. You are right is not feasible to do a Feature Circular bend Pattern
The weight is 815 Gm in Flat Carbon Steel 3 mm Thickness.

The vertical high is 60.091 mm, so is little more the total of 60 mm.
Thanks for your time to model it up. Unfortunately, standard "Circular Pattern" and "Circular Topology Pattern" features do not work with sheet metal specific commands.

I had some luck with "Circular Topology Pattern", as it gives a preview of the result, but it fires up an error after clicking on OK.

topology pattern2.png

topology pattern2 error.png

Let's hope that it would be implemented within the next releases as the preview of the pattern gives us a clue that the software is already working up until to a certain level.

The correct mass is 809grams when the density is set to 7800kg/m3
You aren't too far from it, but not in ±1 gram tolerance though.

@OTE_TheMissile @HaroldL
If I had to model this, I'd designate the top "arm" as the master and drive all the other 3 arms' features through the Equation Editor. Then adjust the length of the inside flanges to get the 60mm height (through some napkin-scribble trig) before tuning the length of the outside flanges to get the 300mm BCø

@tyc , that is an interesting part and although it is a simple one it can be a challenge. It seems the more sheet metal tools Alibre adds the more options that are available for creating sheet metal parts.

You guys came up with the same idea of driving the features through Equation Editor. @HaroldL thanks you so much for an amazing tutorial on modeling the sheet metal part up. I find your screencasts very helpful, as you explain everything very calmly, almost like an educator. Me being a new user of Alibre, I'm still discovering all the cool features that come with it, and it looks like the Equation Editor has a vast range of use cases where it makes designing more efficient and design changes much easier.

This drawing is taken from a speed modelling oriented youtube channel. Although everyone had somewhat different approaches, I think the most accurate and fastest modeling of this part is by using "Contour Flange" command provided the circular pattern works. Otherwise, the speed modelling becomes a real challenge as you have to calculate the lenght of the 60 degree angle flange and bunch of other work arounds.

Well, I think what we can draw from this post is that it is very much possible to model this part in Alibre's sheet metal workspace, with a couple of workarounds which causing longer design time.
 

HaroldL

Alibre Super User
This drawing is taken from a speed modelling oriented youtube channel. Although everyone had somewhat different approaches, I think the most accurate and fastest modeling of this part is by using "Contour Flange" command provided the circular pattern works. Otherwise, the speed modelling becomes a real challenge as you have to calculate the lenght of the 60 degree angle flange and bunch of other work arounds.
Speed modeling - sounds interesting. Would you mind sharing the link?

There is a reason that circular pattern cannot be used in Alibre, if I recall correctly it has something to do with referencing the underlying sketch. Maybe @DavidJ could explain it better.

One thing that this particular exercise demonstrates is that the Contour flange needs to be repeatable in the model, I could see sketching two profiles, 90 degrees apart, and applying a Contour flange on both. I don't know what the programming issues would be but I can think of situations that being able to apply a second or third contour flange would be beneficial in more that this part.

contour flange req..jpg
 

tyc

Member
Speed modeling - sounds interesting. Would you mind sharing the link?

There is a reason that circular pattern cannot be used in Alibre, if I recall correctly it has something to do with referencing the underlying sketch. Maybe @DavidJ could explain it better.

One thing that this particular exercise demonstrates is that the Contour flange needs to be repeatable in the model, I could see sketching two profiles, 90 degrees apart, and applying a Contour flange on both. I don't know what the programming issues would be but I can think of situations that being able to apply a second or third contour flange would be beneficial in more that this part.
Yes, you are absolutely right. It would be helpful if the contour flange is avaiable to use as many times as we want. Currently, it disables after the initial use.
Great thinking Harold!

The youtube channel is called TooTallToby. Click here.
He shows his way modelling this particular part using SW in this video. Please click
 

HaroldL

Alibre Super User
This drawing is taken from a speed modelling oriented youtube channel.
Well let's see how this method fairs for speed modeling the bracket which took me about six minutes to model. One thing that does help, if speed is your main objective, is having pop up menus that come up near the mouse so you don't have to go searching for them in drop down menus or even the ribbon. although the ribbon does help a lot.

Speed Model Bracket.jpg

And here's the video:

 

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tyc

Member
Hi Harold. Pretty impressive. Flange commands aren't actually too clunky at all when speed modelling this part.
You have a good point having the commands nearby. For that reason, I actually quite like the menu which pops up when you left mouse click on an empty space in sketch workspace. Very useful feature by Alibre. Assigning shortcuts for most used sketch objects (like line, circle, center rectangle), even for sketch constrains could increase the speed and productivity in general.

I actually have a small project in mind, building a replica of Elgato Streamdeck with Arduino, where I can assign macros to buttons. Search on youtube "Freedeck" or "FreeTouchDeck" for inspiration :):cool:
 

DavidJ

Administrator
Staff member
Simon, how did you manage to get those bends to display like that for you? Is that screenshot from AD, or did you 'print' the drawing in some way...

I just get solid lines for the tangent edges when I produce a drawing from Harold's file.
 

OTE_TheMissile

Alibre Super User
Yeah my focus has never been getting models/prints out as fast as humanly possible, I lean more towards modeling in ways that are easy to understand if I need to come back later to make changes or revisions.

"Always do a good job for the next guy, because the 'next guy' is you." -AvE

Which is quite literal in my case because I'm the only CAD tech here.

I've also never designed parts to a weight before, even when I worked in aerospace.
 

HaroldL

Alibre Super User
Yeah my focus has never been getting models/prints out as fast as humanly possible, I lean more towards modeling in ways that are easy to understand if I need to come back later to make changes or revisions.

"Always do a good job for the next guy, because the 'next guy' is you." -AvE

Which is quite literal in my case because I'm the only CAD tech here.

I've also never designed parts to a weight before, even when I worked in aerospace.

I agree with you on the "speed" point. When I was working I liked to take my time to make sure the model was easily understood for the next guy and also could be modified when needed for "custom" projects. Of course we had defined processes for that. Speed modeling is a good exercise to see how familiar a person is with the tools available for the job at hand. I think it is used at SolidWorks World when they run their modeling contests. On the job though it can create some issues. Odd too that it seems the models used in the speed modeling contests are rather simple one-piece designs. When you get to modeling complex assemblies it's a different world and the old addage that "speed kills" can take on a new meaning.

We used the weight of a part in order to get the final weight for calculating it for shipping and our procedure was to always add material to each part so the final weight was as close as possible to the physical item or assembly. We didn't include packaging items like shrink wrap, bumpers, or cardboard though. All that was in the final scaled weight.

@simonb65
That image is a screen shot of a drawing using a blank sheet and a default A Horizontal format. The lines you see are the bend tangent lines set to Phantom (.5x) in the Layers dialog. How the lines are displayed is zoom dependent.
 

HaroldL

Alibre Super User
The youtube channel is called TooTallToby. Click here.
He shows his way modelling this particular part using SW in this video. Please click

Thanks for the links. What Tony demonstrates in SW are some of the features that I used in my sheet metal work. He keeps referring to the "S" key which is a customizable pop up tool bar that SW introduced a few versions ago. I kind of liked it and did make use of it. Too bad Alibre doesn't have that, however, it can be simulated with the Space Mouse Radial menus. You just have to create macros for each command you want to add to the menu when you set it up. I don't think they are application aware, by that I mean they don't recognize the modeling workspace and the drawing workspace as separate, they are both Alibre. So commands entered for modeling will show up when the menu is activated in the drawing workspace and visa versa. If you wanted a menu for 3D modeling and one for 2D drawings then it would be best to use the LH key for one and the RH key for the other. Of course I'm talking about the puck shaped Space Mouse

iu


not the one with all the buttons. This one has buttons that, I think, can be programmed.

iu
 
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