Please pardon me as I'm new here and with using Solid Edge. I was wondering what the best way to set my company's title blocks up to auto-populate from the models.
As of now, I have it set up somewhat to take info. from the file properties dialog. It's a bit confusing as I have to use all of the tabs to fill out the properties. Is it possible to do something different where everything can be labled to my preference and located in one place (such as the variables table)?
If anyone could give me some direction on this and point me to some documentation, it would be greatly appreciated.
Solved! Go to Solution.
Sounds like you need to learn about property manager - a modifiable, spreadsheet-like interface to manage properties in assemblies, parts and drafts. Use that instead of the file properties dialog.
I'm looking at it now and not making much sense of it. It's got my model and it's parents listed, but I don't seem to be able to add anything to it.
Hopefully Tickoo's book will come soon and I can figure it out.
FRom SE Help on "property text"
you need to set up property text boxes in your template and then you can use property manager to help you set the properties.
then you can update all property text and your title block with "auto" update with the properties.
It's unclear how much you know but it seems to me you know about populating the drawing format with properties and you're looking for a better way to manage the properties.
Hopefully the attached image will help some. Right click any existing column and the dialog shown will come up. Select "Columns" to turn on or off desired columns, "Show Properties" to add or remove which properties are selectable for the columns dialog.
You can also add new properties via the show properties dialog but I typically don't use that feature.
The light is starting to flicker. Yes, that's what I want to do... Add my own text properties and carry them over to the title block. I'm guessing I can add whatever I want, or am I limited to certain equations within Solid Edge to identify these custom column names? We did this a long time ago at another company with Solidworks, but I can't remember how it worked. Creo Parametric has an identifying symbol (&relation) to show a relation. Is Solid Edge similar?
You can add any property to a text box or callout as Matt (the other Matt) stated. I'm not sure why you're talking about being limited "to certain equations". You can use existing "out of the box" properties or custom ones you create. You can see available properties in the "Show Properties" dialog in property manager or in the "property text" dialog when inputing text.
I did 30 years of AutoCAD, and non-parametric modeling, then a year of solid works before working with solid edge. It is tough getting used to the data base flow structure. Here are the thought processes I use for variables feeding the BOM:
1. Create a single BOM (parts list) format. Then set up your files to feed that single format.
2. Only a single part number and name can exist in each model file. Most use the Microsoft file properties of Title and Document Number for this.
3. There are two pre-established methods of getting cut lengths into the BOM
for sheet metal, Cut X (Flat pattern cut size X or something like that) and Cut Y can display the overall size of the sheet metal flat pattern
for frames there is a cut length.
4. I have created two custom variables set up to be use in the BOM
I use "L" to represent the extrusion length of any shape.
I use "Shape" embedded into any of the "frame" files.
Note: Varaiables must be exposed to be used.....a checkbox in the variable table. To keep say sheet metal variables exposed all the time, expose them in the template file.
Now here is the first point:
I have two columns for all the cut lengths:
Cut 1 displays: Cut X, Cut Length, and L
Cut 2 displays: Cut y
I have a column called material, it displays both the sheet metal gage or the shape variable I added.
The trick here is that the file will only contain of the three cut variables. Placing all three in the column of the parts list makes it work.
The last tricky issues is when you make a model of a single part you fabricate that needs to be both drafted and used on other assemblies. Say I'm making a drawing of a simple angle iron. that drawing includes the part number and name of the material is it made from. I then place that part into an assembly as a place holder for the part number and name of the finished part. The part file is used for drafting. the assembly is used to insert the part into another file.