I would just create it as a hatch pattern in the drawing.
Depending on the level of detail you are looking for there are a couple of approaches.
If you want to show the physical representation of the insulation in your drawing, you will need to create a part. One piece of insulation is not an issue. If you are representing the insulation in building construction, I think this effort would grow rapidly.
If you only require a notional representation in your drawing, but you want the BOM to show a proper handling of it I would suggest creating a virtual part in your assembly with no features. Edit this virtual part and set the custom properties to represent the insulation. Create an additional custom property called something along the lines of "Quantity Required" and put in the amount needed. At the top of the custom properties window set the BOM Quantity drop down to your "Quantity Required" custom property. The Assembly BOM will then use this value in the quantity column.
In the drawing, use some sort of sketch entities to represent your insulation such as Troy suggests. You can attach a ballon to this sketch entity and it will show a "?". Click on the balloon again to edit it and in the property manager you will see a list of non-visible parts to choose from and your insulation should be in this list. It will probably be the ONLY thing in this list. Select it and your balloon will now show the line number in the BOM corresponding to the insulation.
A final approach is to just create the sketch entities in your drawing with a note as outline by Troy.
Thank you both!
I want to create a snake/loop like pattern that is often used in the contruction industry. The hatch pattern for solidworks regarding insulation is just dottted lines however.
Do I and can I create a custom pattern?
Thank you all who helped.
Scott, your post lead me to searching around the internet for patterns and more forums as to how to get this batt insulation into Solidworks.
For anyone who is wanting to add batt insulation pattern to solidworks, here are the steps I have done:
Go to Solidworks directory (may differ):
1. Save a copy of the origional Sldwks.ptn for saftey
-make sure to change file extension so Solidworks doesnt read both files
2. Open file Sldwks.ptn with notepad or wordpad
3. Scroll to bottom, under last pattern entry
(each begin with a "*"), copy and paste following:
*:501:ISOLANTE, AUTOCAD BATT INSULATION
161.57, 1,1, 7.59,2.53,-56.92,6.32
18.43, -1,1, -7.59,2.53,-56.92,6.32
108.43, 1,1, -20.24,2.53,18.97,-44.27
71.57, -1,1, 20.24,2.53,18.97,-44.27
*501 is the beginning of the number sequence solidworks has defined as user patterns.
*In the Sldwks.ptn file there are instructions on how to edit this code if desired. Also the name of the hatch pattern "ISOLANTE" can be changed
Glad I could help you. Thank you for not only posting your results, but the forumla
for this as well.