I have a welded assy which is going to be machined (assembly cuts), what is the best way of showing the model in those two states (unmachined/machined)?
I have had this problem for years. I have a casting and a machined part, both have drawings. "HOW DO I DO IT" I ask PTC. Answers ... no idea ...... This problem must be one of the most BASIC ones to deal with, yet I still have no hard fast rule.
Having tried MERGE, ASSEMBLIES, SUPPRESSED FEATURES the only one that 'works' is using the evil 'FAMILY TABLE' option. Hence:
Generic: Machined part
Instance: Casting (Raw part)
I have no intralink, so its works OK.
(I have to use the BACKUP and SAVE_AS commands to do up issues ... but thats another story)
It depends-if you are using the bill of material feature in Pro/E, then make a part out of you casting (.prt), and an assembly (.asm) that uses the cast part as its only bill item for your machined part. This way, the bill of material integrity will always be kept.
You can add machining features in assembly mode, although rounds and chamfers on your machined surfaces will have to be made as "cuts" or "protrusions" and you will not be able to color-code your machined surfaces, if your company requires that.
If you do the machined part from a merged part or from a backup or save-as of your cast part, your machined casting will be a part (.prt) and will not have any bill items associated with it. One way around this would be to add your casting part number as a parameter, which you can then attach to a (3-D) note.
You should use either the Master Model merge technique or use inheritance features.
for Master Model:
create an assembly with all the component parts to be welded. Assemble an empty part.
Merge all of the component parts into this new empty part.
open the part and add any machined features(part level).
create 2 simp reps, one with all component parts, one with only the merged part.
Use the simp rep with the components to drive the BOM.
Add a view of the simp rep of just the part to show the finished state.
For inheritance:
create a new part, use feat>creat>data shar>inherit open each component and bring it in.You may need to add some datum features like csys to assemble them correctly. After each is in you now have access to all of the original features in the model tree, you can make them variable or not and add cuts etc.
Learn more at
Hi,
The exact scenario that you are describing - parts that need to be represented in their pre and post machining states,is described in detail in Pro-Files magazine.
Issue: Spring 2002,Vol.6, No.3
The article is called "Design Using Inheritance Features"
Several years ago I designed the stator and the rotor of a hydropower unit (14 meters diameter). I had the same problem: assembly cuts. I didn't find a good solution to satisfy all the client's criteria to replace the assembly cuts. The only thing I did was that I increased the RAM of my computer from 500 MBytes to 1GBytes. And the result was spectacular.
You must know that assembly cuts are killing Pro/Engineer (and not only). But, for far, this is the best approach of reality.
If your computer is able to handle this complex calculations, go with this method. If you choose any other methods (family tables, simplifird reps, merge etc) you'll have a lot of trouble with naming conventions and bom table. And I do not mention here the headache of the person who will need to modify the design and you are not there...
I'm not working with 2001 version and I do not know what inheritance feature is able to do.
My advice: Improve your hardware (especially memory) and go with assembly cuts.
We haven't started using ProE 2001 yet but I've tested the inheritance feature in 2001 and it seemed to be a good idea for cast parts.
But for a welded assy the inheritance feature can not be used, its base model have to be a part.
Sorry to say but none of the suggestions have got me excited and said that this was the way we should do it.
Maybe PTC should make the inheritance features be able to have an assy as its base model.
Thanks to all which have participated with tips, and please feel free to add additional tips.
From my understanding of your question, I think that I've been doing this for quite some time now. I don't use a family table for this operation. First, change color of all part models to white, or any color you choose that would best represent a machined surface. Next, change color of ALL SURFACES of each part to a different color. What this does is show the machined surfaces in a different color so you can differentiate more easily. It's kinda like peeling a potato! Then, create the unmachined assembly and save it as a part number. With your new assembly, create the machined cuts and the white surfaces are then revealed. With all your assembly cuts in, save this new assembly as a new part number.
This way when you create your bom on your unmachined assembly drawing, it will include all the parts that went into the assembly. And when you create the machined assembly drawing, it will include just the unmachined assembly with all the machining processes.
Hope this helps. It's worked for me for years without any worries. I don't use Intralink, just a folder for all parts and assemblies.
I was actually looking for help to the cast/machine dilemma in Pro/E for myself.
I have tried each of the methods that have been suggested thus far and my experience (~2 years) is that it depends on what you are trying to accomplish with the casted (pre-machined part/assembly) model?
1) If you use an assembly model (.asm) to create the cast part you satisfy your BOM, but you are limited to only a few of the cut features available in part mode. 2) If you use a family table and create an instance for the casting and each machined part you have to deal with PDM issues regarding family tables. 3) If you use the merge technique you may run into the problem, which I have many times, where the reference to the merge needs to be modified and you have to redo the reference merge and reroute every feature to get the machined part to resolve. 4) I am still investigating the inheritance feature for the cast/machine scenario, but only time will tell.
Your problem is a little more in depth than mine, since you need to show machined cuts on an assembly (more than one component). If you were to use the merge function you are limited to a single component as reference and a part model as the destination. Therefore, you would need to create your pre-machined assembly, use it as a sub-assembly and then perform the merge with reference to your machined part. However, you would notice that the pre-machined assembly (when cross sectioned) is detailed as a single entity. All surfaces that mated or overlapped in the assembly would now be one surface. Perhaps you can live with this result?
I know that I have not helped you with your specific problem, but hopefully I have shed some light (as everyone else here has done) on the subject of cast/machine parts in Pro/E.
We have had very bad results using assembly cuts. All the features were created, everthing worked & regened, the drawing was made & saved but on retrieval it all failed to regen. Days of work lost.
The merge works well for us. I can change the initial component parts and it shows up in the merged part. I can add all the cuts I need to the merged part to get the final product. You can work around the BOM problems with empty parts to fillout the BOM.
have you tried with pro/program? If you define a variable "machined"- for example- so if it's not true supress all the machining functions the only thing you have to do is regenerate the assembly changing the value of the variable. The trouble is that in drawing you can't have the two models at time. You must regenerate to change from one state to another.
Create simplified rep for the part: (exclude/include features you need)
e.g. "rep_machined" and "rep_unmachined" for cast.prt
Within weld assembly, create simp-rep, "rep_machined_assy" to include cast.prt. Select "replace" command for cast.prt to choose the "rep_machined".
Create a dummy assembly. You can name it what every you like. Assemble your un-machined part using default datums. Let's say your part is 123-456.prt Now create a new part and name it 123-456_m.prt The m is for machined. Now go back to the assembly and assemble 123-456_m.prt to the assembly using default datums. I know that it only contains datums at this time. That's ok. Now do a merge and select the machined model as the model to perform merge process to. Then the original for reference parts for merge. Now you have two models. One is the original un-machined part called 123-456.prt and if you open the 123-456_m.prt model you will notice it looks identical to the original. You can now perform all your machined cuts to the machined model and it will not effect the original model. You can now make two drawings or one drawing with two pages for the un-machined and machined versions. The great thing is that if you make a modeling change to the original part, it will trasfer the change to the referenced merged part. This way they are always updated and the same.
