Hi all,
Im hoping someone can help me with an issue that I have with Inventor. I will give an example first in order to understand the problem better. Say I have 5 cars that are all similar, and they all need to be manufactured, but for this i will only model one car. Then on the assy it will give the quantity for all parts that make up one car. But I want to change to quantities on the single part drawing so that it shows the quantity for all 5 cars. Is there an easy way of doing this besides writing a long code? For example can I change the project iproperties to 5 and then all the quantities in the project file will change to 5 off? We do not stamp our drawings so want to find a quick and easy way to change it.
Kind regards,
iUser
Solved! Go to Solution.
Solved by iUser. Go to Solution.
If I understand you correctly you want to use an assembly model, but in the drawing representing that assembly model you want the BOM to reflect a version of that assembly that is 5X in quantity then what the actual assembly model is?
If that is the case what I an thinking is make an ipart factory out of your assembly model with 4 more assemblies added. Then in the just have the BOM be reflective of the 5X version from the factory.
I hope this makes sense.
If this solved your issue please mark this posting "Accept as Solution".
Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!!
Hi
- In your Parts list Create two new properties of your own choosing.
- I called mine "***" for assembly. (Language Filter blocked it, see pics)
- and "TOTAL" for Total QTY.
- Remove the QTY column from the parts list
Set the column width of "***" to 1, this hides the column from view. (Language filter, see pics)
In the TOTAL Column, I changed the name to QTY
Click on Substitution
Enable Value Substitution, see pic.
Once you place the Parts list, you will HAVE to edit the parts list,
Expand the **** column so that you can see it, add the value of 5 in each row.
The Total QTY will populate automatically and correctly.
Create a stand alone assembly file and put in it as many assemblies of the car as needed. Name it say - Car Parts so you know what it is for. Then in your drawing file when creating a Parts List - select that very assembly file for reference. Turn the visibility off for the parts you don't want in the drawing.
That should do what you are after.
Best Regards,
Igor.
Thanks for the help rhasell, this info already helps a lot! I was wondering if it is possible to create a form for when you start a new project that asks you for the qty of the final assembly? In this case as in the example I would type 5 in this form. The reason is when we start a new project and the customer comes after the job and says he wants 8 more of these, the assembly is already designed and all the drawings done I dont want to manually go and change the quantities on each drawing? We talking about over 500 parts for each project, so is it possible to change the form then and then the quantities throughout the project changes accordingly? I am willing to try the coding / iLogic out if there is a way?
Hi Igor,
Theoretically this does work, but isn't there an easier way about it? Rhasell sulotion seems a lot faster already but there is still a lot of room for error. If I use your sulotion our backup file on the server will grow at very fast rate as each projects file size will increase by say 5 as in my example. And we need to keep these quantities so I cant go afterwards and delete the other four assemblies. See my reply on Rhasell mesage?
Kind regards,
Hi,
Frankly, I wouldn't do it the way you want it to get done. How many drawings are there for one machine? If you want to indicate quantities of the parts on the drawing for each and every purchase order - then you will be busy flat out reprinting them again and again.
It is not a big deal to control the quantity of parts needed for any particular order. For the large items - they can be easily counted. For the loose parts - it make sense to make a few more in case one get lost somewhere. Besides, if it is a repetitive order - then what seems to be a problem with keeping parts in stock?
Anyway, all of my drawings show the quantity of parts needed for one assembly only. And I yet to see it creating a problem down the truck on the workshop floor. But to answer your question if the assembly file size gets large and large with every save - no, it does not. I have just run a quick test on the assembly with 175 different items in BOM (the quantity of parts required to build the unit is close to one thousand). With only one assembly in the file - the memory foot print is 195 kb. With five - it is 225 kb. It is nothing to worry about at all. One other thing - you don't have to delete unneeded assemblies from the file. Just mark them as Reference ones. Reference items do not participate in BOM. Yet you can always change Reference status to Normal one, should the order change.
Best Regards,
Igor.
Hi Igor,
There are between 500 - 1000 drawings per machine, and all the machine are custom built. The reason for not wanting to put the quantity of the parts for one machine is that the drawings get sent to different dept. and we also out source. So the total quantity needs to perfect else it causes problems. Changing it on each drawing becomes time consuming, but looks like we will have to go that route. We did want to write a code that keeps the total quantity of final assemblies with the project file, but the problem is that if you change it, then Inventor does not know to go open all the drawings and to change it. So what we did is created a form that is linked to the iProperties project data. And the we used Authority as quantity. So if you open an assembly or new part you need to fill out this form each time and then the drawings quantity link is changed to authority and then it updates automatically on opening the drawing. Still a lot of room for error but this will have to do for now.
I just wonder how that situation is handled by automotive industry? Maybe you can implement something of similar to what they do?
Regards,
Igor.
Hi
I ran a quick test of creating a Number field in my BOM. I then set the the first one to 5, using drag and fill I copied the value to all parts in the assembly.
Using the Parts list method in my previous post, I replaced the manual field (AS*) with the new field, and used this as the multiplier. It worked as expected, but still not 100% solution for you. (Using the field from the assembly will remove the issue of manually typing the vaue into each and every drawings parts list, time taken to update all values will be a few seconds)
You will obviously have to copy the new Parts list style to all the drawings for the first time though, that could take a while. (Resource transfer might help)
Using this method, you will still have open the thousands of drawings to update the Parts lists.
I do have a piece of code that will do a total qty of parts/sub assemblies contained in a GA, and link it to a customised field, this field will automatically be populated on all parts/assemblies. Perhaps you could modify it to suit your needs?
What you are looking for, I do on a smaller scale, so I have been looking for ways to remove human error.
http://forums.autodesk.com/t5/Autodesk-Inventor/Multiple-sub-assemblies-in-a-Parts-List/td-p/4342872
Gavin Bath
MFG / CAM Technical Specialist
Design and Motion Blog
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Found an exchange app that does exactly what I have been looking for :-)!!!
This app runs through your assembly giving the correct quantities for all you parts and assemblies. It also has an option to specify the quantity of the master assembly making production a lot more simple!
"Thanks for the help rhasell, this info already helps a lot! I was wondering if it is possible to create a form for when you start a new project that asks you for the qty of the final assembly? In this case as in the example I would type 5 in this form. The reason is when we start a new project and the customer comes after the job and says he wants 8 more of these, the assembly is already designed and all the drawings done I dont want to manually go and change the quantities on each drawing? We talking about over 500 parts for each project, so is it possible to change the form then and then the quantities throughout the project changes accordingly? I am willing to try the coding / iLogic out if there is a way? "
Hi there
Do you still need help with this, I have finally got down to making an iLogic code to do this automatically?
I tried the addin that was menstioned in this thread, personally, I prefer my method.
Pleasure mate, glad to be of assistance.
P.S. Welcome to the forum 🙂
Hi,
I am looking for a solution like that with the form and the Bom updating after changing the qty.
Would you please post the full solution.
Thanks
Hi! Do you mind being more specific? Is it about PartsList in a drawing or BOM in an assembly? Could you share a simple example of what you are looking for? I think it is doable but I want to make sure your requirements are understood correctly.
Many thanks!
Hi
thanks for replying,
I have achieved what I wanted using this rule:
Dim oDrawDoc As DrawingDocument oDrawDoc = ThisApplication.ActiveDocument Dim oPartList As PartsList oPartList = oDrawDoc.ActiveSheet.PartsLists.Item(1) oASSQTY = iProperties.Value("Custom", "JOB QTY") ' Iterate through the contents of the parts list. Dim i As Long For i = 1 To oPartList.PartsListRows.Count oCell = oPartList.PartsListRows.Item(i).Item("JOB QTY") oCell.Value = oASSQTY Next
Please have a look to the screencast
I have been able to run the rule by pressing apply in the form.
There is just one problem: if I close the form with the red X button, the new value of the ipropiety "Job Qty" is updated but not the column in the Part List.
I would like to be able either 1 to run the rule on the closure of the form via red X button, or 2. Delete the red X button of the form to close the form only pressing "Apply"