Is that supposed to happen?
Block 1 under sketch 8 should be fully defined because I used the fully defined sketch tool.
As you insert block in sketch. So you need to give dimension to fix the block position.
Hope this will help you.
People use that?
Is Sketch2 correct? (I see multiple issues.)
Sketch5 missing two Tangent Relations?
Well, I am shutting down for the night - so I will go ahead and point out the "issues" that I saw.
Hopefully you have had time to try to discover them yourself on you own.
In this image it appears to me that you missed a snap to endpoint on the left side.
On one side you dimensioned the parallel distance as 0.20 and on the other side you dimensioned the horizontal distance?
This would not result in equal width straps. I suspect that you meant to do the parallel distance on both straps.
But 0.20? That is really really skinny for a helmet strap?
I set the dimensions to display out to 8 decimal places and see this.
These dimensions cannot be measured on the shop floor and therefore cannot be manufactured.
Do not use Fully Defined Sketch except for very very rare cases.
A beginner should probably never ever use Fully Defined Sketch - the beginner needs to learn how to properly define a sketch.
You should by typing in logical Dimensions and using logical Relations.
It's hard to see where on the strap you found those problems.
I'm going to set the decimals to 6 places from now on to make sure I don't accidentally make dimensions accurate to the subatomic level.
I didn't notice the sides were different lengths. I'll fix that.
I normally don't use the fully define sketch tool, but those sketches won't be manufactured. I just need something to use as a mate reference and using planes didn't work for some reason.
Thanks for your constructive criticism.
Here's what happens when I try to mate with the planes.
EDIT: it looks like there's too many problems with this. It's probably just best to make a new set of straps. I found those uneven dimensions and tried to change them, but it just causes errors.
ric Eubanks wrote:I'm going to set the decimals to 6 places from now on to make sure I don't accidentally make dimensions accurate to the subatomic level.
ric Eubanks wrote:
I could not work that way???
Simply enter logical dimensions and problem solved!
Would it cause problems to do it my way? I've always intended to use logical dimensions, but sometimes I miss a few.
If you are a one-man show and always will be a one-man show with one-off products that you will never look at again, then do it however you wish.
However....once you start involving other people in the design process (this includes yourself in the future), you are going to need to be able to give them clues as to why you did what you did. Why does that edge on feature 7 move when I move feature 3? Oh, its because it was dimensioned that way. Therefore it was intended to be that way. There was a dependency purposefully developed because this edge on feature 7 always needs to be x distance from feature 3.
This is called design intent. If you are dimensioning without design intent, you are breeding chaos. If that dependency was unintentionally developed.....then when the next guy/gal comes in to look at it.....what is he/she to think?
This is why Mr. Mather pushes fully defining your sketches even at the beginning stages. The more you do it, the better you will get at it. The more you do it, the more developed your eye will be for spotting things.
And regarding your "set the decimal to 6 places" comment. Well....every single dimension that you put into a sketch should be entered logically. 25.00001 is NOT the same as 25. Even if you can't measure the difference in real life.
Take this as an example:
Its a silly example, but the point is, if you were to extrude that shape and then try to use it in an assembly, the program KNOWS that the top and bottom faces are NOT parallel. Therefore, you will be adding in extra work to mate this item into your assembly. In addition to this, you will also be creating a stack up of issues if all your parts are like this.
Manufacturing is NOT an exact science. That is why there are tolerances. However, CAD IS an exact science. And should be treated as such.
Start practicing drawing your sketch way outside where it needs to be, then adding dimensions and bringing it back. This way, you will be sure to get exactly what you want.
Eric Eubanks wrote:I've always intended to use logical dimensions, but sometimes...
Eric Eubanks wrote:
I've always intended to use logical dimensions, but sometimes...
Here is a part downloaded from a "reputable" site.
What issues do you find with the design?
Solidworks is really easy to learn, but you are in for a whole new challenge when you start fully defining everything. For me it was harder to learn how to fully define everything than actually learning the basics of the software. I wasn't aware of a "fully define sketch tool". I think I'll check it out but I don't have high hopes for it ;P. Plus once you get good at fully defining sketches it becomes really fast and easy. Second nature. And if you don't know what needs defining, just move blue lines around with your cursor and you will figure out what needs to be dimensioned.
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