I have several dimensions. Especially curves that don't do anything when I try to dimension them with smart dimension. How do I add dimensions for those lines and curves?
Apparently they are treated as splines, circles or radius's cut on an angle will give you that effect.. Can you turn the part so you're looking directly at the sketch the feature was built from and then dimension it from that view?
Do you mean an auxiliary view?
You could say that..
I can't find a good reference edge for what I want to do. I also tried relative view. I'm not sure how that works.
In the part file you can select the sketch and hit normal to view and then hit the spacebar and save the view as a new view (name it), then go back to the drawing and insert the part and pick the newly saved view to insert..
If you modeled this part then you hopefully made all your sketches fully defined. All of your drawing dimensions are grey colored which tells me you added them one-by-one in the drawing. Instead I recommend you use Insert -> Model Items (at the very top).
I marked the settings to use, but you should read up on this and all its options in the Help. (The circled icon on the left is just to show where I keep this icon on my toolbar and what it looks like.)
This is such a fantastic tool as it puts the dimensions you used in your sketches right onto the views of the drawing. You will have to move them around and maybe even use the Shift button to move a dimension or callout from one view to another, but it allows you to use right there in your drawing the very same definitions you used to make the part. It also helps to keep from overlooking some dimensions, which is very easy to do when manually creating dimensions.
If your views or sections are off for any reason you can get a spline that you cannot dimension, as John has pointed out. But if you defined your features with dimensions in your sketches then it makes sense to re-use that work in the drawing.
I learned about that in the tutorial. I wasn't sure how reliable it was.
Eric Eubanks wrote: I learned about that in the tutorial. I wasn't sure how reliable it was.
Eric Eubanks wrote:
It never fails! Seriously, try it and only supplement the drawing with manually created dimensions when something was defined with geometric constraints in its sketch, but you need to communicate it on the drawing.
Additionally you can add sketch points along curves in your parts and show them in your drawing, dimension to them, then hide them again. If you do this make sure it is obvious what the dimension means. And, I'll add that my suggestion is a last resort.
What dimensions would I need to add manually as a supplement? Does the model items not add every needed dimension?
Eric, the Model Items are the dimensions that you used to make the part. They are as you've molded it, you sketches.
So that means if all my sketches in the part are fully defined it should give all needed dimensions? It would seem like that would happen, but I see lines especially curved ones that aren't dimensioned.
This is the updated version using the model items
It is reliable. Word of caution as you being new. If you change an imported dim on a drawing your model will change to the new dimension as well.
When I am working with an intern this is the last suggestion I make for 2 very good reasons.
1.) Easy to change a model without meaning to.
2.)More important in my book, if you detail parts and get used to making a drawing that makes sense (how is this going to be made?). It gives you the tools to approach design from the perspective of how am I going to detail this?
I am not saying you can't use your model dimensions. Just putting in my 2 pennies on someone who is new to the software and design in general.
Don't underestimate Dennis's suggestion. The whole point of SWX should be to convey design intent. If you define your parts with the correct dimensions, tolerances, surface finishes, processes, etc., you can have that intent carried into your drawings.
Take a look at this part:
How would you model this? You have choices. But, for this part the best way to model it may be how they are going to build it:
Especially notice that the rope grooves are "cut" in my model below. If you model this way, you can get accurate weights and such from the actual steel that will be used. If I were to produce the grooves as a revolve, you can't get that information by rolling back the model.
I hope this helps.
Can you handle such a groovy wheel
looks good btw
You would think so, but this is not the case. If you grab the view that the sketch happens to be parallel to, you can get all of the dimensions from that sketch into that drawing view.
In this drawing I had to create a "View" in my part that was parallel to the plane the circled hole was on to get the view to show this hole:
This was not for a production drawing, I threw this together for a colleague yesterday. That view to the left should be clarified. I probably shouldn't be showing you bad drafting, but I was trying to show my point.
Most likely, yes.
So, some of those lines might be projections of other lines that you'll see when looking at certain directions at the part.
Actually, I can't handle that wheel, it has a 10'10" diameter rope pitch... I'd need a crane...
Here's one from a previous bridge:
And thanks for the compliment. I did it pre-SSP and it has a lot of work into it, such as FEA and bevel cuts for welding. If I get time, I'll design it in place, SSP style.
This already looks much better. But here are few drawing quality comments.
1. First drawing appears ISO. This one ANSI. (The ANSI looks better, IMHO.)
2. 100.00 and 10.00 degrees. How about only one or zero decimal places on these.
3. The two .71 dimensions should probably be a 1.42 diameter dimension in the front view.
4. Top view: Pull the extension lines off the object lines. The .04 dimension and R.08 cross each other. This is a no-no. Also, what does the .04 tell us? I suspect it is a bad way of indicating a radius.
5. Is there draft on this part? It looks like it but there is no dimension or note for it.
6. The knob profile in the right side view is missing a radius.
7. The 1.18 dim in the front view should be a diameter.
8. Three standard views is preferred because it is sufficient in most cases. However, I suspect you will need a back view and maybe a section view for this part. I suspect there are features on the back that are not visible here and therefore not communicated. Remember, you have to look at the drawing as if it is the ONLY piece of information you are providing. Does the drawing really have everything they need to make the part?
There are more, but it is clear to see you are learning and getting better.
I'll give you this advice again because this would be a very good part to use just your drawing and its information and make a brand new model of this part. No fair using the previous model, just use the information on this drawing. That will tell you a lot about what information needs to be on the drawing and will help you figure out what is missing.
You never answered my question to you the other day about what texts or other resources you are using for this class. Please list them for us.
The photo looks like the part is a weldment. I suspect also the blank was a casting. How are you actually making the part?
Just me and wonder if anybody else see's it. But are there not dimensions on there that are almost impossible to measure to.
You don't want to have your angles to 2 decimal places.
Go into your drawing template and set your tolerances:
Once you are finished, click on Edit Sheet:
And save your new template back to the location that you drawing templates are saved:
I went ahead and modified a drawing template to get you started.
David Nelson wrote: Just me and wonder if anybody else see's it. But are there not dimensions on thee that are almost impossible to measure to.
David Nelson wrote:
Just me and wonder if anybody else see's it. But are there not dimensions on thee that are almost impossible to measure to.
Honestly, if we could get it forged, we'd really like that. But I never got a clear answer on how expensive it would be, or if it was even possible. The compromise has been to get the hub and ring as an ASTM A668 Class D S4 forging and the stiffeners and web as plate steel. However, because this is put out to bid, I'm going to include an option to have the whole thing forged, or at least the hub, rim and web. And we'll see if the foundry I was in contact with is competitive.
Here's a clearer picture showing the welds:
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