Drawing Dimensions Question

Hi, everyone!

I am wondering if it is best practice / "obligatory" to always use the dimensions of the provided drawing, or if it does not matter as long as the end result is exactly like the drawn part.

Here, for example, I have carved out the part piece by piece, not using all the dimensions of the drawing, but rather inferred new dimensions from it. Is that OK?

On a side note, I threw away the 12CAD manual that was flooded with mistakes and lacking dimensions, and I now use an exercise manual from TKMCE that can be found here if anyone is interested.

Figure6.SLDPRT

Figure 6_JD_Sketches.SLDPRT

Your part is fine.

There are often more dimensions given than are necessary for symmetry.

Use logical symmetry about the origin - that will be important when you get to assemblies.

As much as practical - avoid sketching on part faces - sketch on origin planes instead.

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Your part is fine.

There are often more dimensions given than are necessary for symmetry.

 

Use logical symmetry about the origin - that will be important when you get to assemblies.

 

As much as practical - avoid sketching on part faces - sketch on origin planes instead.

Mather, your part is of enormous pedagogical value to me, thank you so much!

May I ask you why we should avoid drawing on surfaces?

Also, by origin planes, do you also include planes added by reference geometry, or preferably just the very first three planes?

Akitrija, I don't follow the same methodology as JD. I don't find problems drawing on planar faces, but you just have to be careful and sure of your dimensional references.

Something to understand about sketching, and feature creation in Solidworks, is that you can have varying degrees of open and closed contours in sketches, and your features can be offset from the sketch plane. This means you can do things like sketch a rectangle and extrude a "thin" version of it or you can sketch a rectangle with 4 circles in it, extrude the rectangle with no holes from the plane, then extrude just the circles starting from the extruded face.

The very important things are really making a fully defined sketch and using relations when possible. Things like construction lines, = relations, perpendicular instead of a 90degree angle etc. My guess is that JD doesn't like sketching on faces is because the geometry is able to change, while a plane(unless defined off a face/vertex/edge) would inherently be more stable. When possible make things symmetric about the origin and always be aware, when you apply dimensions, how things will update.

Akitrija, I don't follow the same methodology as JD. I don't find problems drawing on planar faces, but you just have to be careful and sure of your dimensional references.

 

Something to understand about sketching, and feature creation in Solidworks, is that you can have varying degrees of open and closed contours in sketches, and your features can be offset from the sketch plane. This means you can do things like sketch a rectangle and extrude a "thin" version of it or you can sketch a rectangle with 4 circles in it, extrude the rectangle with no holes from the plane, then extrude just the circles starting from the extruded face.

 

The very important things are really making a fully defined sketch and using relations when possible. Things like construction lines, = relations, perpendicular instead of a 90degree angle etc. My guess is that JD doesn't like sketching on faces is because the geometry is able to change, while a plane(unless defined off a face/vertex/edge) would inherently be more stable. When possible make things symmetric about the origin and always be aware, when you apply dimensions, how things will update.

Thank you for your answer, shift1313. This means that IF I am careful with my feature relations, for example "up to surface" in stead of "blind", sketching from surfaces would not generally create problems later if I choose to change the part, right?

As you get into complex geometry - you will often find a need to edit earlier geometry in the feature history tree.

These edits can cause later sketches to "go sick" if based on part faces rather than origin geometry.

On most of my parts (even, or especially, very complex parts) you could delete all (or most all) of the features without any of the sketches "going sick".

This is called the Base Orphan Reference Node (BORN Technique).

Akitirija, yes, BUT some things are inherently more stable. For instance if you can use "Up To Next" in place of "Up To Surface" it will be more stable. This is because up to surface can vary if you make edits to features used to create it.

Example, if your surface was made with a revolved sketch and at some point you want to change it but can't make it happen by simply editing the original sketch and need to add a spline, or arc or something. The face ID(what solidworks uses in the background) is now different and the feature will fail. You can edit and reattach it to the new face but it's just a headache usually. If "Up To Next" works it doesn't care if faces or features change.

As JD mentioned with the BORN technique you can get away from sick features BUT with more complex parts i rarely find ways that i can reference original sketches as opposed to edges, vertices or faces. Because when you start to make complex 3d geometry it tends to get farther away from the base sketches. You have to pick your battles and really its based on what types of things you design.

my suggestion is just to be familiar with as many options as you can. If you can always get away with sketches on standard planes then go for it.

Hum, I think I understand more or less what you are saying. Thank you very much!

It would be easier to explain with an example modeled multiple ways. There really are so many nuances to parametric modeling.