What you are doing there is far more complicated that what I'm attempting.
The best example I can give at the moment would be creating weld neck flanges.
I envision having:
1. Part file with multiple configurations.
2. A master drawing file.
3. Individual drawings for each size required.
It's simple to do, you could use:
- Drivework Express (The best solution)
- Global variables
- Design table
As you can see in pressure vessel you change:
- input / output changes
- Diameter of the outer cylinder
- Ammount of tubes
- Diameter and length tubes
- Section of reinforcement rings
- Quantity Fixes to civil foundation
If you have a few variables you can do it, You're wright with your variables of your project, show me something and maybe I can make some suggestion
Just a thought, why not to use DriveWorks Xpress and generate part when you need it?
I'm not familiar with DriveWorks Xpress, but I'll look into it.
The goal at the end of the project is to have drawings completed for all of our standard sizes, so I not sure if "generate part when you need it?" works for what I need at the moment.
A configured part/assembly with a single drawing sounds good. I've seen a lot of drawings where the variable dims are simply given a letter designation and then a card with the actual values is printed out for each job.
If you do 2a and lock drawings to a particular configuration, remember that those 'lock' at the level of what is used in the drawing. Consider making a pack and go and 'locking' an entire folder at the end of your project, and keeping every thing in the folder as 'read only' on your network so nobody makes changes accidentally.
Richard Ahlgrim wrote:
2a. If I create individual drawings is it possible to “lock” a drawing to a single configuration?
Yes, you can select which configuration each view is set to.
In your set up drawing, create your views and set them all as "link to parent" (except the one driver view). Then run your save as, and you can just switch the config of the main front view and it switches all other views.
It will depend to a certain extent on your needs. I'm working on a project now that has 6 installation variations, and will have all six shown in a single Drawing. I created six configurations of the model, inserted a drawing view, along with one projected view, one section view, and two detail views. When I had that just the way I wanted I copied and pasted the sheet, changed the parent's referenced configuration, which also updated all the other views, and repeated until finished. If you can have all in one document I don't see any reason why that wouldn't work.
However, I suspect you need separate Drawings for each configuration. If that's the case then after getting the first drawing finished you could "save as" the Drawing, and change the referenced configuration. By using this method you'd have a single model with however many drawings there are variations.
You asked about "locking" a Drawing to a single configuration. If by that you mean you want to remove the ability to change the configuration that a drawing view is referencing then I'd suggest doing a Pack and Go of the first Drawing, creating a new Part and Drawing with new names. Repeat as many times as needed, change the references as needed, and then delete the unused configurations from each instance of the Part. By using this method you'd have a separate Part file for each Drawing, and since each Part would only have only one configuration it couldn't be changed in the Drawing.
Thanks Glenn, I think the "save as" method might work best for this particular project and be the best / closest fit to the way we typically do things.
Locking the drawing to a single configuration would be nice but not a real requirement. We are small enough I don't too much concern about others mucking about with finished drawings.
Now that it's been mentioned the Pack and Go method would work great for creating non-standard one-off versions of the part.
I haven't made a series of drawings as you describe, so these are opinions and not tested advice.
(3.) You can also create one drawing, with a single sheet for each configuration. Fully create the 1st sheet, dimensioning to common geometry which changes per config, and then copy the whole sheet and choose a different config in subsequent sheets. The dimensions ought to update to the new geometry once you change its configuration.
Be sure to use config specific properties to drive callouts, titleblock info, and whatever changes on the drawing between configurations.
It's up to you whether you reference sheet numbers, as a multi-sheet drawing representing a single part may be sheet 42 of 123 instead of 1 of 1. To me, I'd think one multi sheet drawing would be simpler to manage than 1 drawing file per component (created with Save_As..), but what's easier for you probably depends on how you'll be releasing the drawings.
I am unclear if you'd be taking it further in this direction, but:
Another commonality you can create for more interchangeability between similar but different models is reference entities. If you have a second part similar to the first, you can create PrimeAxis, EndPlane, FacePlane, or DiamTangentPlane (or w/e works for you) and then only dimension to and between those objects in the drawing. Then, you can Replace Model to change the part in the drawing, and it should automatically provide references between the same entities still attached. Some extra attention in the part creation can make repetitive drawings easier through common references (aside, the same can also apply with parts in assemblies with Replace Component).
I love this forum!
Thanks for all the replies. This place really is a wealth of knowledge with a lot of cool folks willing to help whenever asked.