Assembly comprised of multiple components all derived from the same master sketch "4 Inch Rail Master Sketch"
Using the sketch to drive geometry, using the parameters to drive various extrude lengths.
Geometry changes seem to propogate quite well, while parameter changes do not...is this a bug or am I doing something wrong? Generally have to open each individual part and "edit derived part" to force changes to propgate...
Or is there a better way to accomplish what I am trying to do?
files attached (move end of part marker down for all .ipts).
Thanks for any help!
Solved! Go to Solution.
Solved by johnsonshiue. Go to Solution.
Welcome to Inventor forums,
We will need your version of Inventor to better help you..
Inventor Professional 2014 - 64 Bit
Build 170 Release 2014 RTM - 02/28/2013
BTW. I didn't intend to attach all 3 zip files!
ALDoor contains all needed files, but all EOP's are rolled up.
ALDoor1 and ALDoor2 each contain half of the need files but the EOP's are NOT rolled up..
Hi! Could you walk me through the exact steps to see the problem? Which parameter in what part to change?
Thanks!
Question, did you derive them from within the sketch part, or did you start new parts and derive them from them? If you derived them from inside the sketch part, you will need to open those derived parts up, select the top level entity in the browser, right-click and choose update. If you start a new part and derive them, they should update automatically.
To be honest I dont' recall which method I used... Is this intended behaviour? Or is it a bug?
In order to get the other partsd to update you have "Edit derived part" on each part...
Are you trying to make multiple parts from the same original, just different dimensions? If so try this. Copy your original in case of mistakes 🙂
Open the copy, go to the Manage tab. Under the Author subtab select Create iPart. A table will show up at the bottom with all preset parameters. If you need one not included, select it from the top left. You may then right click on the table and select Insert Row. rename these however you want. Change any parameters to the values you want. When you have all the rows you need select ok. When you place this single part in your assembly, a window will pop up giving you the choice of which size to place. No need to keep track of 20 versions, one part will allow you to add any size.
its not that hard, just go slow at first and you'll be up and running in no time.
Editing the original table will change any existing parts to those new values, unless it's a name change.
Although if you are making seperate parts from one master component all different is shape, size etc, I would not use derive. I would use the Make Part option or Make Components to put multiples into one assembly. They can be placed in an existing assembly, or into one created then and there. Or just made as parts to be placed later. Experiment with those two options, these parts made this way will automatically update whenever the original is changed. If you use the Make Components option it will place them all in a new assembly in the exact same position as your multibody parts. You will just need to rename the solid bodies to your part names in the multibody parts for tracking purposes, otherwise your parts will be called Solid1 etc. Although in the next step you can rename them, it just makes it easier to know which solid body belongs to what part if you rename the solid bodies in the original part. Include any parameters (export) that you want included in the parts.
Hi! Many thanks for providing the detail steps! It saves me a lot of guessing. I think I might know why this behavior happens. Indeed, it is abnomal when changes in derive source part does not get propagated to derive part. However, there is a problem with the derive source part.
1) Open 4 Inch Rail Master Sketch.ipt and go to Parameters dialog.
2) Find "leafheight" and look to the far right column.
Export is not checked.
This checkbox needs to remain checked if you want the update to propagated. Do you recall why it was unchecked? If you don't remember how it was unchecked, there could be a workflow changing it from checked to unchecked. We need to find out how it could have happened. Otherwise, I assume it was unchecked manually. When the checkbox is unchecked, any further change with the paramter will not be pushed to derive parts.
To fix it, you simply check the box. Then go to each derive part referencing this parameter and edit derive part node and hit OK. Now the update should work. If not, please let me know.
Thanks!
That was it!
While I've got your attention can you tell me if fundamentally one of the methods below is more or lest "robust" than another? (Less likley to break, less computing intensive, faster to update etc...
I am speaking primarily of using these methods for driving parameters / formulas
1.Create new part, - derive from existing (using one part as a "master parameter source" then derive it into multiple parts
2. use "link parameters" from another ipt or iam instead of derive
3.use "link excel"
Hi! Among the three workflows, I don't think one is less reliable than others. They go through similar code path. The behavior should be similar. In your case, the key to lead to the problematic behavior is due to the fact that Export flag was unchecked. Did you recall how the flag was unchecked? Did somebody uncheck it manually? Or, it somehow got unchecked automatically? If it is former, the resultant behavior is expected. If it is latter, there is a problem somewhere and we need to find out how to reproduce the behavior.
Many thanks!
I beleive it is because the parameters in question are "User Parameters" I just went in and created another use parameter and by default the eport box was unchecked upon creation.
Thanks for your assistance!
Unfortunately I faced same problem
I have a big assembly with rules forms and derived parts from source sketch
after renaming my sub folder with vault I recognised same problem !
I ticked export check box in my first source part in its parameters table
Auto update not working !
I have to go through each individual part edit derive part and click on the sketch and press ok
It will update just onece and still auto update has got big problem
any perfect solution ?
Found the solution to my similar problem (Inventor 2020)!
I had updated my master sketch with a new Work Plane, then when going in to my part, the sketch does not auto update with the new Work Plane (even after rebuild all).
If you right click the master sketch & edit derived part, you will see that the new Work Plane is there, it just needs the green plus applied!!
It looks like it is the same fix for paremeters etc.
As you can see by the half green half grey circle, you can dig down to see which items have not been included...