This shouldn't be difficult at all. BOM's can be easily linked to a specific drawing view, pulling the needed info from said view, so that when the view changes the BOM will update. Can you explain how you're going about setting things up? Have you made drawings in SolidWorks before? If not, check out the tutorials under 'Help'.
Unfortunately i dont have much experience with SolidWorks drawings, as i usually use UGS NX. However, I HAVE tried the automatically generated BOM. The problem with using this, is that i need it to change according to rules in driveworks. For example, the language / name of the parts should change according to who is generating the order/drawing. There is also other things, like the color of certain parts should be in the item description etc, so when the user changes the color, the description also changes.
While I'm not 100% on the language portion, everything else is possible to do for sure. The thing is, it's not just a quick thing to explain. You need to be well versed in DriveWorks and SolidWorks. Where you have experience with NX, I'm guessing you can pick up SolidWorks fairly quickly; at least the portions you need to know. Specifically, getting the BOM to populate with the data you want/need. I'd strongly suggest you look at tutorials, the ones within the software as well as those available on the web. Short of getting paid training, these are your best options to complete your project.
If you are using a SolidWorks BOM table, you can do one of two things, both involving cusstom properties. First, you can use the special custom properties that SolidWorks provides. If you drive the custom property DESCRIPTION in each of your parts, then that description will be inserted into the BOM. The other option is to create your own custom properties (again, on each part, not in the drawing) and change your BOM columns to display that custom property.
DriveWorks can quite happily drive custom properties. In the Capture Utility (the part of DriveWorks that runs in the SolidWorks Task Pain on the righthand side) when you're capturing features and dimentia to drive, you can also capture Custom Properties (look towards the bottom of the screen). We will typically set a rule for a custom property to be something along the lines of:
=Concatenate(DWVariablePartType, " WIDGET WITH ", FinishReturn, " FINISH AND ", DWVariableOptionalFeature)
This just builds up your description from control values or variables.
The important thing to remember is that the description is INTELLIGENCE ABOUT THE PART/ASSEMBLY, and as such, it should live there. SolidWorks allows you to create as many drawings as you want of the same model. By putting the intelligence into the MODEL, then each of these drawings will automatically pull out the same information each time.
Hi and thank you very much for your help. I didnt have any experience with solidworks coming into this project, so i didnt know much about custom properties. This helped a lot
I still got a couple of problems however:
1 (Important) : I have a part in my assembly that i DONT want in my BOM. Lets call this part A. I have 8 of these "part A" in my assembly.
It was easy enough getting rid of the As in the original drw file. (They all appeared in a single row with a qty of 8. I clicked on the arrows to the left of the BOM, right-clicked part A, and selected "Exclude from BOM"
However, in my driveworks project i am creating (driving) all 8 different As. (A1 , A2 etc) and substituting them into my final assembly. This makes all the As reappear in my BOM (on different lines). How do i permanently get rid of the As ?
2 . I would like driveworks to autocreate balloons for the parts in the BOM. I`ve tried a few different things but cant get this to work at all. The closest i got was attaching the balloons manually to all the parts in the BOM. This works fine if i keep the exact same parts in the final assembly. It also works to delete a part ; The balloon is automatically removed. HOWEVER, as soon as i try swapping one of the parts for another, the corresponding baloon gets "unhooked" and will appear in the middle of the drawing.
I guess it just doesnt know where to attach the balloon, since the parts dont share any features. I could try to put in a dummy feature in all the parts, and attach the balloon to this.
Any help would be greatly appreciated
I'll answer your questions in the same order you have asked them:
1) Your issue here is that you are telling a Drawing sheet to exclude the As when they are not actually there in the original Drawing. Therefore in your master and the 'A' parts are no longer there, your command to 'Exclude from BOM' becomes obsolete. There are two possible solutions to this:
A) Instead of subsituting all the A's into your final assembly, have them actually there, so that they appear in your master drawing (with the different part names, i.e A1,A2 etc.). that way when you remove them from the BOM, SolidWorks will know which parts you are referencing to.
B) Use a General Table, instead creating your own headings, and by either manually typing in the part names, or by linking the fields to the custom properties which can then be driven through DriveWorks (the same way as Paul Gimbel mentioned above).
2) This behavior is regularly seen with DriveWorks. When you are swapping parts, the balloons will become unhooked- this is called a dangling dimension. To hide these, you will need to go to your Master Drawing, and set the document settings to hide the dangling dimensions. How to do this can be found in the Help File below:
However, this means that when you swap in the part, that balloon will disappear. To resolve this issue, you will need to manually replace the part inside SolidWorks, and then open the master drawing. With the newly swapped in part visible, you will need to attach a new balloon annotation to that part. You can then go back into the model, revert the swapped part back to its original, and then save both your model and drawing. Now, depending on which model is active, the corresponding balloon will either be shown or hidden.
If you would like to control the text in the Balloon, you will need to click on the Balloon in the master drawing, and change the 'Balloon Text' section in the SolidWorks Task Pane from 'Item Number' to 'Text'. Once done, you can then capture the balloons annotation text, and set a rule inside the model rules to drive the text.
I hope this information helps.
Hi and thank you very much!
Yes this does help a lot. Though its more work up-front to swap in all the possible parts (There is quite a few) than i hoped for. Is there any way for driveworks to run the "Auto balloon" feature in Solidworks ? I do have DW Pro, if that makes a difference.
Another option regarding the balloons is to create a drawing inside the Master Assembly, on a Plane that does not disappear during generation. Then draw a sketch point on the plane in approximately the region of where the swapped in parts will be, and then fix this sketch point.
You can then go into your Master Drawing, turn on the ability to view sketches, and attach the balloon to the sketch point. This way that sketch point is always there, and by using a rule to drive the numerical value inside the balloon, you can control what value is used depending on what part is swapped in.