They're not exactly identical. The volume is only 0.04 inches off in the mass properties. Is that a big deal? I did notice a few needed changes to my drawings from this.
In other words, your drawing failed to communicate the necessary information to properly make the part, resulting in something being made wrong...scrap. Out in the world, making things wrong is not a profitable venture. So, in a nutshell, it is a big deal. This is why people recommended that you do it. It is how you can cross-check your work. It is how you find problems (as a student/learner) and become better. In the end, every time you create drawings for something, you will be cross-checking your work in your head...making sure the information presented will make it exceptionally difficult (ideally, impossible) for anyone to follow the print and make the item wrong.
Ok I'll see what I did wrong.
Double check your significant digits - I see a lot of people use .38" when it should be .375"
(that adds up really fast!)
p.s. I haven't downloaded/reviewed the models yet.
Just downloaded the parts - fillets are different, there is a fillet missing, and units are different.
(Units being different can very easily cause the "rounding error" that I mentioned.)
Your first extrude is off by .112" because of this.
Missing fillets and fillets that are the wrong size can be a very big deal.
Speaking as someone who uses both models and drawings to produce machined parts every day, Todd is absolutely right.
Your models need to be exact. More and more CNC programmers and machinists are putting toolpaths directly on the models. If the model isn't correct, the part won't be correct without the user correcting the model or program which adds cost to the part.
I just made a drawing this morning from a model that came with a "limited dimension" drawing.
On the supplied drawing there was a dimension with a 5.996mm / 5.896mm tolerance. The model was 6 mm.
That may not seem like much but there were several adjacent angles and fillets. When the toolpaths are put on the model and the resulting code input into the machine tool the part doesn't come out right without a lot of tweaking which again adds cost.
I could give you many examples like this, some much more severe but the moral of the story is make your models exact. In the long run it will reduce the cost of the resulting parts.
Sorry for the lecture. Bad models are a pet peeve of mine.
Is it a big deal, yes.
1 piece discrepancy is a big deal and here is the simple reason why.
You made the part based on a drawing. You could not achieve the design intent based on said drawing. Therefor your objective was not met. This may sound harsh, but I and others here deal with this on a daily basis.
"Use my model to make the part the drawing is just rough dimensions." *See this alot*
1 piece not too big of a deal, how about an assembly with a tolerance stack applied at the assembly level of varying degrees? If 1 part is not controlled how do you control the final stackup? Will your assembly even remotely work?
Eric you are asking the right questions. The one downfall I see every day is interns and cad operators who focus on a part rather than an assembly. Even demonstrations at VAR meetings challenge with what is the most complicated part you have ever made? I challenge back what is the most obscene totally kick ass machine you ever designed? Because at the end of the day a part is only as good as the machine it help built or the assembly it helped construct.
The units conversion issue aside - this sort of things falls into my, "Can't you see this bucket?"
The OP will need to develop an eye for geometry.
Differences like this need to jump out like a Gazelle in the grass to a Lion. Instantly catch attention.
I was having a real hard time figuring out what I was looking at from the section view until I opened the part. Once I opened the part it was crystal clear. I come from the 2D drafting world and all of those tangent edges confused me. I'm asking if this is something that should be removed or do people keep those tangent edges? I think it seems a little clearer if they are removed. What does someone with a little more experience with this think? Eric, don't do this until someone a little better qualified answers, but I think this looks a little clearer:
Though there is still a tangent edge visible, I can quickly see what is going on from the above image.
At my place if I am working on an old drawing I put back in Tangent Lines. The reason is the parts just do not look right.
... especially when he starts working with really complex geometry.
The different sized fillet and missing fillet on the thru hole jumped right out of my screen.
Eric Eubanks - Attention to detail is a really big deal, and the faster you can spot subtle differences, the better off you will be . . .
Showing/not showing tangent lines is a function of clarity more than policy at most places. My tangent lines are shown by default, but as phantom lines. We hide them if that helps to make the drawing or part easier to understand by removing clutter, but in most cases we show them as phantom lines.
Ok I see the missing fillet on the hole. I have the fillet in the drawing, but it's just shown as a circle. How to you specify that it's a fillet in the drawing?
The fillet that J. Mather pointed out is on my drawing. I must have missed that. Looks like interpreting drawings is something I need to work on.
After trying to fix the rounding errors because the original was in millimeters and the rebuild was in inches I still can't seem to get them to have the same mass properties. Does anyone else see how these are different?
Again the attention to details will bite you in the arse. Overlay the 2 models on top of each other in an assembly. This will help looking for discrepancies. In this screen shot one diameter is 54.06mm and the other is 54.1mm. Details, details, details
I noticed one looked smooth and one looked more pointy. I just didn't know why.
that is merely the graphics of your system. I highlighted each edge to confirm what my eye caught by looking at what showed up in the bottom right corner of the screen.
This is not from your parts of course. But a quick glance here can save you later down the road......
How did you find the diameter of those? I can't find it with smart dimension or by editing the sketch.
This will save you a lot of frustration -
You don't always have to use the units of the model when changing a dimension.
The units are inches, but you can type in a metric value like this, and SOLIDWORKS will do the conversion for you.
Eric Eubanks wrote: After trying to fix the rounding errors because the original was in millimeters and the rebuild was in inches...
Eric Eubanks wrote:
After trying to fix the rounding errors because the original was in millimeters and the rebuild was in inches...
You can enter mm units in an inch model - SolidWorks will take care of the conversion for you.
If you are doing an inch drawing of a metric part - set your number of decimal places to 3.
like I said above, select the edge and look in the bottom corner of your screen. It should be there.
I just noticed for some reason one model has dimensions like 0.2 and the other had dimensions like 0.1968486542.
This really illustrates what we are all talking about here:
The I.D. was 1.97in, but you will get the "true value" if you type in 50mm - it should be 1.9650394in
(I don't know about anybody else, but I would rather just type in 50mm.)
The little stuff adds up really fast, and attention to detail is extremely important.
I would use the "Tangent Edges With Font" setting in this case. Solid tangent edges are just not useful to me, and only serve to cause confusion. Just my preference.
That sounds like you have your decimal places set differently in each model.
I don't know how you got 10 decimal places though. I can only go to 8 decimal places.
I just typed a random number for that.
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