Drawing with visible dimensions.

[papajoe41]

Hi there,
I have been using Alibre Design for a while now and enjoying what it can do. But, there is one thing that is bothering me. When I make a new part and put dimensions on it, why do the dimensions disappear, when saving the part. Once the part is saved, when I call it back up, the dimensions are missing. I have to click on the 'sketch' and hit 'edit' for them to show up. I have tried to make a 'drawing' from a 'part'; but, the same thing. When I submit a drawing to a company to do an estimate. The dimensions should be right there on the submitted drawing. As a machinist, when I was given a drawing, it always had the dimensions on it. Is there a way to do this?
Thanks,
Papajoe41

 

[HaroldL]

How are you creating drawings?
Have you watched the Drawing training videos? These are for Alibre Design Pro and Expert and are a bit dated but they still give good information.
The dimensions that you use to control the size and location of sketches are "hidden" along with the sketch when the feature is created.
You need to create dimensions on the drawing if you want to know what those feature sizes and locations are.

 

[simonb65]

When I make a new part and put dimensions on it, why do the dimensions disappear, when saving the part. Once the part is saved, when I call it back up, the dimensions are missing. I have to click on the 'sketch' and hit 'edit' for them to show up.

Dimensions in 3D sketches are only there to help you create the sketches as part of the solid modelling process. That's why they don't show when your not directly actively editing the sketch.

When I submit a drawing to a company to do an estimate. The dimensions should be right there on the submitted drawing. As a machinist, when I was given a drawing, it always had the dimensions on it. Is there a way to do this?

Dimensions lines and callouts in 2D drawing need to be added and placed as part of the drawing creation. You don't need to enter lengths for those dimensions, Alibre knows what they are. You just need to place the dimension lines using the dimension tool between two points/edges, etc. Alibre will add the length/diameter/radius/etc ... as explained in the training video @HaroldL pointed you to!

 

[Jim T.]

So you have to physically put every dimension on the drawing that you want to be on there?
I'm pretty sure the other programs I've used, ProE/Creo, SolidWorks, Catia all SHOW the dimensions in the drawing that were utilized to create the parts/assemblies.
This is like having to enter every dimension twice, once on the part/assembly, and again in the drawing.
Someone please tell me this isn't the case!

Jim
AD Expert V24

 

[DavidJ]

No, you don't enter dimension values twice.

Unless you've chosen to include design dimensions in the drawing (which often looks a mess) you do have place dimensions in the drawing, the values of which populate automatically.

 

[HaroldL]

As @DavidJ said, if you include the design dimensions in the drawing you don't have to add any dimensions on the drawing. I have used SolidWorks and have opted to use the design dimensions, and true to what @DavidJ mentioned, it is a mess, or worse. IF you are going to use design dimensions to annotate the drawing then, as you create the part, you need to plan the placement of the dimensions in the part so they show correctly on the drawing. That can be more work than just dimensioning the drawing with the drawing dimension tool later. Another point, I don't know if you follow any drafting standards, but using design dimensions on the drawing usually don't follow the prescribed standards very easily.

And here's another issue that you need to deal with when using design dimensions:

 

[Jim T.]

So you're saying DON'T use the dimensions that you created the parts/assembly with? I use dimension standards religiously including GD&T. What I don;t understand is that if you don't use the dimensions that you created the parts with, how is it parametric? How do the parts and the assembly update if you edit a dimension on the drawing that you annotated on the drawing ie a reference dimension?

Thanks
Jim

 

[DavidJ]

Simply because the 3D design, and the 2D drawing are linked. The size is already fixed, so dimensions placed in drawing get filled automatically.

 

[DavidJ]

If you need to edit size, you can 'edit 3D design' from the 2D drawing.

 

[Jim T.]

So any annotations that I make in the 2D drawing will update the 3D model, even if the dimensions in the 2D drawing aren't the same as the ones that I use to create the 3D model?

 

[DavidJ]

Any DIMENSIONS will update, yes.

 

[Jim T.]

I need to create elevation dimensions for buried tanks under ground. When I created the assembly, I created an assembly data plane at ground level, then placed all of the tanks and other equipment referencing that datum plane so that I could illustrate how deep the contractor should bury the tanks. I have a front and top view in the drawing, the front view is where I need to show bury depth. How do I annotate the bury depth without a physical entity to dimension to? All I have up there is a datum plane that doesn't even show up in the drawing.

 

[OTE_TheMissile]

I need to create elevation dimensions for buried tanks under ground. When I created the assembly, I created an assembly data plane at ground level, then placed all of the tanks and other equipment referencing that datum plane so that I could illustrate how deep the contractor should bury the tanks. I have a front and top view in the drawing, the front view is where I need to show bury depth. How do I annotate the bury depth without a physical entity to dimension to? All I have up there is a datum plane that doesn't even show up in the drawing.

I keep a model of a tiny sphere in my CAD library for those rare occasions when I'll need to have a print reference something that I haven't actually modeled. It does nothing but provide a place to generate a point I can dimension to in my eventual Drawing (center of a circle), but because I have it included at the Assembly level I can constrain it to be parametric with the rest of the Assembly.

Two or three of those constrained to your ground level plane ought to do the trick.

 

[NateLiquidGravity]

So any annotations that I make in the 2D drawing will update the 3D model, even if the dimensions in the 2D drawing aren't the same as the ones that I use to create the 3D model?

I think you were getting confused. Only Design Dimensions let you change the model from the 2d drawing.

 

[Jim T.]

Sounds like an unusual work-around, but OK! I understand exactly what you're saying to do, and I don't hear anyone else saying "That's Crazy", so that's what I'll do.

Thanks all in this chain, I know I'm asking alot of questions and believe me I look for the answers before I bug you folks, but time is of the essence at the moment as well!

Have a great weekend everyone!!

Jim

 

[Jim T.]

So any annotations that I make in the 2D drawing will update the 3D model, even if the dimensions in the 2D drawing aren't the same as the ones that I use to create the 3D model?

I think you were getting confused. Only Design Dimensions let you change the model from the 2d drawing.

- Nate "Liquid Gravity"


Any DIMENSIONS will update, yes.

DavidJ

So I guess there are differing opinions on this? I would like to be able to edit the dimensions on the drawing and have the assembly model update automatically, so I would want to use Design Dimensions? How do I get them to show up on the drawing?

Jim

 

[OTE_TheMissile]

I'd never heard of Alibre until I started working at this job & pretty much spent my first two weeks rubbing the keyboard against my face until it did what I wanted it to, then I found these forums. That was back in, 2008? 2009?

Stick around, these folks'll get you sorted

 

[HaroldL]

so I would want to use Design Dimensions? How do I get them to show up on the drawing?

As much as I don't use design dimensions I understand there are some that do. The easiest way to get them into a drawing is when the drawing views are created by expanding the More Options tab of the view creation dialog. You can also RMB click on a PART view and select from the mouse menu to Reproject Design Dimensions. I don't see either option available for an assembly view.

 

[OTE_TheMissile]

To be perfectly honest, looking forward I think you'll want to get used to the idea of editing the dimensions in your models and pushing the changes to your drawings rather than the other way around.

 

[DavidJ]

You could model a chunk of ground, either just a slice to show ground level, or a larger piece, perhaps sitting behind the tanks.