- Create a copy of the part and edit as required
- You may create configurations in the same part.
- Copy and paste the sketch from one part to another.
- Save the sketch/feature as library feature and use that in may parts as required.
Think I have a similar problem to Tim's original post, which is giving us some issues while preparing to implement a PDM system
We make tyres and need to link the mould profile sketch from our Mould Plant drawing to become the tyre outer profile in multiple design drawings, while keeping the links between the 2 live so we don't change a mould without updating all the relevant tyre design drawings
looking at Deepak's response,
- creating a copy & Copy & Paste
which is what we have historically done has caused several issues with moulds being modified without updating all associated design drawings
- Configurations within one part
gets confusing when you have several different designs for different projects within 1 drawing
- Library feature
is sort of what we want to do, but in creating the library feature we still loose the link to the master drawing and we would have to maintain this for all our moulds
What I really want to be able to do is import a sketch from the mould (model) drawings as a reference link into our design (model) drawings
Any thoughts would be greatly appreciated
Chris Valentine wrote:
What I really want to be able to do is import a sketch from the mould drawings as a reference link into our design drawings
Is that a 2d Drawing OR 3d Model?
Sorry, yes its the sketch from the 3d model in the part file I want to copy across
As others have stated, you need to use in-context modelling wither thru an assembly OR part into part.
You may be able to make an assembly with the two parts. Then create the sketch in the "driving" part (sounds like your mould). Then choose "Edit Component" on your "driven" part. Then you could select the plane in your "driven" part and the sketch from the "driving" part in the feature tree. Then you would go to Insert>Derived Sketch:
This would link the two sketches together (make sure to fully lock down the driven sketch, it has two degrees of freedom once it is created). If you make a change in the driving sketch it updates in the driven part.
You have to be careful if you go this route because using in-context relations can cause trouble if you don't manage them well.
Good luck and let us know what you come up with.
try to do some incontext design work then. Create an assembly with the two parts. From there you can use the same sketch from the other part by converting entities. When you change part A part B will update also.
the other thing that you can look at is inserting parts into your parts. This will allow different file names and should keep the ref files updated.
Save the Sketch as a Block and insert the block into the new file and extrude... Or if it's a part with a series of sketches then I would save the part (with only sketches, which I call a Skeleton Sketch Part) and work within an assembly creating a top down design method.