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Drawing import

SOLVED
JustinSauber
Newbie

Drawing import

Creo 2.0

M090

 

I have created a model where I used an inheritance of an existing model.

This is similar to how our supplier will handle the manufacture of this part.

If part A exists in stock remove from stock and add holes and it becomes part B.

 

I created a second page to my drawing where I have imported part A's drawing. I did this so that in the event that part A does not exist in stock the supplier can make the whole thing from scratch. This helps the supplier avoid:

-Making part A removing from machine

-Placing it in stock

-Taking from stock and putting back in machine to create part B

 

Now to the real question/concern:

 

I feel that the import drawing/data on page 2 is just a snapshot and will not update if changes are made to part A drawing.

That being the case the designer will have to import this any time either model changes.

Is there a way to have this auto update or is this just wishful thinking on my end?

I am open to suggestions on how to improve my current method.


Regards,

Justin


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1 ACCEPTED SOLUTION

Accepted Solutions

Re: Drawing import

Justin, in your attempt to save time you may have created more work.

An efficient method really depends on how you manage the component files.

I would say that from what I can glean from your description is that you have a "gray" part that requires secondary machining for which you already have a part drawing. Then you have a finished part as an assembly that adds a secondary operation to complete the part... or you have an intermediate assembly to create the inheritance in order to add features your assembly cannot manage. And for this finished part you also have a drawing.

Now you want to add a sheet on how to make the part from scratch. You have two options that I can see:

1. finish the part in your original part and make that the master for a family table. Remove the additional features as a family table instance. Report that instance to the assembly that creates the inheritance component.

2. make a completely new part (save-as the gray part) and finish it. In the drawing for the finished part, add the model and complete the drawing using the new model for subsequent views.

As in many things Creo, you have to plan these things. Often, company policy tells you what you need to do, but when you have the freedom, in this case, I would use family table instances (which I rarely use!) I have no love for merge/inheritance parts. I don't even touch a drawing until I have the models set. it drives me batty when a manufacturing engineer just willie nillie changes the entire product structure after all the drawings are finished. I provide plenty of opportunity to provide input before I start drawing.

Drawings are great about letting you add multiple models and they also handle changing reference models in the views reasonably well. I always save a printout of what I have just in case everything blows up.

I am from a background where managing BOM structures in the assembly structure (and PDM) was important. Non CAD people determined how they wanted these structures. This was my guiding principle for how a model was created and documented. A choice such as gray=>finished compared and from-scratch has always tripped up PDM systems. I first look there to see how they resolved this and try to copy this technique in CAD. The next question of course is what part to use in the next level assembly. one of the two becomes orphaned, in a sense.

Regardless of how you manage it, yes, you want to maintain associativity in the event an ECO affects the part -anytime- in the future. This is why I recommend the family table at the part level. There is almost no way anyone can overlook the existence of two instances in the drawing.

I just went through a part that had 4 levels of secondary operations. Assembly cuts wouldn't work as I needed to deform the part at the 3rd level. This included 3 subsequent unique drawing levels to follow. It was a nightmare to manage while developing the methodology because I was learning and doing on the fly and it really tripped me up. Once I got it settled, it maintained consistency and I have no doubt it can be sustained in the long run.

Welcome to the forum, Justin.

View solution in original post

4 REPLIES 4

Re: Drawing import

Justin, in your attempt to save time you may have created more work.

An efficient method really depends on how you manage the component files.

I would say that from what I can glean from your description is that you have a "gray" part that requires secondary machining for which you already have a part drawing. Then you have a finished part as an assembly that adds a secondary operation to complete the part... or you have an intermediate assembly to create the inheritance in order to add features your assembly cannot manage. And for this finished part you also have a drawing.

Now you want to add a sheet on how to make the part from scratch. You have two options that I can see:

1. finish the part in your original part and make that the master for a family table. Remove the additional features as a family table instance. Report that instance to the assembly that creates the inheritance component.

2. make a completely new part (save-as the gray part) and finish it. In the drawing for the finished part, add the model and complete the drawing using the new model for subsequent views.

As in many things Creo, you have to plan these things. Often, company policy tells you what you need to do, but when you have the freedom, in this case, I would use family table instances (which I rarely use!) I have no love for merge/inheritance parts. I don't even touch a drawing until I have the models set. it drives me batty when a manufacturing engineer just willie nillie changes the entire product structure after all the drawings are finished. I provide plenty of opportunity to provide input before I start drawing.

Drawings are great about letting you add multiple models and they also handle changing reference models in the views reasonably well. I always save a printout of what I have just in case everything blows up.

I am from a background where managing BOM structures in the assembly structure (and PDM) was important. Non CAD people determined how they wanted these structures. This was my guiding principle for how a model was created and documented. A choice such as gray=>finished compared and from-scratch has always tripped up PDM systems. I first look there to see how they resolved this and try to copy this technique in CAD. The next question of course is what part to use in the next level assembly. one of the two becomes orphaned, in a sense.

Regardless of how you manage it, yes, you want to maintain associativity in the event an ECO affects the part -anytime- in the future. This is why I recommend the family table at the part level. There is almost no way anyone can overlook the existence of two instances in the drawing.

I just went through a part that had 4 levels of secondary operations. Assembly cuts wouldn't work as I needed to deform the part at the 3rd level. This included 3 subsequent unique drawing levels to follow. It was a nightmare to manage while developing the methodology because I was learning and doing on the fly and it really tripped me up. Once I got it settled, it maintained consistency and I have no doubt it can be sustained in the long run.

Welcome to the forum, Justin.

View solution in original post

Re: Drawing import

... or 3. you can simply fully detail the merged part on a new sheet and treat it like a from-scratch part

Wouldn't be my 1st choice.

Re: Drawing import

Antonious,

Thanks for the quick reply. Adding the model to the drawing didn't even cross my mind. Thanks for the reminder as I had forgotten about this functionality.

Re: Drawing import

Gotta love simple solutions

You might mark your own answer as correct since this is much easier to read.

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