Driving assemblies with a sketch 1

[Scott4tg]

We make door panels of all different sizes and configs. I know there is a way to make a layout sketch in an assembly and then insert each part of the door and have the length of each component driven by the layout sketch. Can someone point me in the right direction. We want to have an openening for the door assembly say 60" wide and 96" tall. We would like to put in each each part, the bottom, top and side but have their individual lengths mated to the sketch dimension so that if we want to change a width or height we would just have to change the layout sketch.

Thanks in advance.

Scott

 

[josephv]

Hello Scott,

One way to do this is via equations.

For example, in your layout sketch create a dimension called "height@layoutsketch". Then make the height of the panel and opening equal to "height@layoutsketch".

This way when you update your layout sketch the parts will also update.

cheers,

 

[Eltron]

The layout sketch option is available in '08. When you create a new assembly in the Begin Assembly dialog pick Create Layout, and a 3D sketch will be born. This will be the layout sketch that you are looking for. Also, check the Help for Layout Sketch.

Dan

http://www.eltronresearch.com

 

[Adrian2]

Hi Scott;

This is very easy to do using Solidworks Weldments.

I use them frequently for structural steel frames and even for wood framing.

When you say doors I am assuming you are talking about residential or commercial doors where you have standardized jambs, extrusions, headers and sill plates and so on.

All of these items could be defined as library feature parts and placed in the weldments where required, although you could also sketch them in and use configurations for all the different sizes of doors.

The nice thing about weldments is the simplicity of the sketches and the lack of need for lots of equations. Everything is tied to geometric relationships to the original sketch.

Best Regards


Adrian Dunevein
AAA Drafting Services

http://www.aaadrafting.com

http://home.cogeco.ca/~adunevein/

SW2006 Office Pro. SP4.1

 

[TheTick]

Using sketches to drive assemblies is nothing new. Very effective for top-down design.

If you use a top-level sketch to drive parts, I recommend you have a second "sub-master" sketch in each of the components that drive features from the top-level sketch. By this, I mean create a master sketch at the top of each component that copies the elements of the top-level sketch you will need, and then use the component=level sketch to create features. Do not drive part features directly from your top-level master sketch.

The reason for this extra layer is to make your models more robust. If you need to "reconnect" in-context references, you will only need to do it in one sketch per component, rather than in multiple features. It will also make your part files easier to manage later in the product's life cycle.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[TheTick]

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http://www.esoxrepublic.com/models/>

The hinge model in "Hinge.zip" uses top-level sketches driving master sketches in components like I discuss above.

 

[drawoh]

Scott4g,

Just do it! I am not aware of anything that would stop you, other than perhaps your boss.

Make a sketch in the assembly. Attach the sketches and features of your parts to the assembly sketch. I draw optical schematic sketches all the time.

This is how you control the dimensions of the parts of an assembly from a design table. You can use equations to drive your sketch, but equations can drive your part directly.

JHG