I am not sure if FOP will do this. I would like to have a part that can change in size when used in different assemblies. for an example, i want a 1" diameter tub to be 6 inchs long in assembly "A". but i also want this same part used in a different assembly "B" but i needs to be 12" long. Maybe i want to use the same part in the same assembly but i need each occurance to have a different length. how would i do this?
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It kind of depends on what you want to do with the BOM.
You can do basically what you describe with "Adjustable Part". The part sizes itself based on the context of the assembly -- but it will have the same part number in each context. This approach is good for springs.
If its really a Tube and you want to have different part numbers depending on length, then "Frame" might work well for this. Frame only works for extruded things - like tubes and structural steel. but it lets you choose what constitutes a single roll up on the BOM;
1. All like sections are same part number. or
2. All like sections and length are the same part number or
3. All like sections and length and exactly the same cuts/adds (i.e. exactly the same body) is the same part number.
I found another way of getting this done.
First off I already have two columns in my parts list called Cut 1 and Cut 2.
Cut one display sheet metal Flat pattern cut size X and the length of frame members
Cut two displays sheet metal Flat pattern cut size Y.
I also set up Cut 1 to display "L"
if I go into any part, and add dimension L or edit say, extrusion length variable to L, then L will display in the Cut 1 column.
You can take this a step further, and format the display of "L" after the name property.
I also embedded a system to display X, Y and Z for when the same concept is used in 3 Dimensions. In this case I re-name plane position to X, Y and Z.
What would make all of this easier is the addition of a concept I call string math. Take a look at what can be done with document name formula. To bad that property can't be displayed in draft. Also the ability to link and update variables from files names would help this out too.
Using ordered and plane driven parts (The part sketches start useing includes from plane, and all other dimensions refer to the plane includes). The plane position then control the part and the parts list display as described above.
What I have yet to figure out is how to get the part to re-size bassed on how it is mated rather than a hard input number.
This is exactly what FOP & FOA is used for. First you need to create the Tube. Then create a FOP for it. Using the FOP table, change the length of one of the tubes to a different length. Now you have two parts with different lengths that make up the FOP.
Next set up the assembly. Create a FOA. Create the two intances you need. Using the FOA table, "Replace" out one of the tubes with the other tube.
Our entire operation is run like this. All of our parts have dash numbers (like screws, the dash number represents the length in inches).
To my understanding FOP/FOA use a file for each instance. I need the one file to change that add another instance. Very long story why. Short version....downstream math is required and complex to set up.
Actually, FOA does not have to populate a file to be used like FOP does.