Easy Question for an Expert

[MattP]

How do you bring assembly features (i.e. extruded cut thru multiple parts)into a part drawing? Or...how do you bring those features back to the part file? Is it possible?

Thanks,
Matt

 

[speedy12]

Because you are creating assembly features, they are only in the assembly file and the assembly drawing. If you make a drawing of the component part, it will not have the assembly features. As far as I know, you cannot move a feature from an assembly to a part. You can always put the feature in the part and dimension it there with the default values and then once you have it in the assembly modify the dims to position the feature where you want it. If the feature is dependent on features in another part that is in the same assembly, you can leave the sketch underdefined and use relations to define it in context.

 

[MattP]

OK, maybe I am going at this the wrong way. What I would like to do is create a hole pattern that matches mutliple parts. I don't want to have to make these features for each part. Maybe there is another way to do this.

It seems like there should be a feature somewhere in a part or drawing file like "Import Assembly features". Seems pretty simple to me. Maybe I should just write my own CAD software...OR I could learn the CAD I use.

Matt

 

[MadMango]

Look at Holes Series in Help. I think this is what you are after.

Ray Reynolds
"There is no reason anyone would want a computer in their home."
Ken Olson, president, chairman and founder of Digital Equipment Corp., 1977
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[MattP]

Thanks Mr.Mango. That is basically what I am looking for. Now, does that only work with the hole wizard? What if I wanted to make an extruded cut, i.e. square hole or keyhole shape?

 

[MattP]

Yeah, I know how to do all that. I just want to make the cut one time for all the parts and have these cuts show up in the part file. I'm pretty lazy I guess.

 

[MattP]

Oops, where did youare74's reply go?

 

[rockguy]

Draw the sketch in the asembly file and then edit the parts in context of the assembly. Create the cuts in the part files and refrence the assembly sketch you created. Then all parts are driven off the one assembly sketch.

 

[MadMango]

Hole Series only works with Hole Wizard. If you need non-Hole Wizard features to propogate through your assembly parts, you'll have to do as [blue]rockguy[/blue] said above.

Ray Reynolds
"There is no reason anyone would want a computer in their home."
Ken Olson, president, chairman and founder of Digital Equipment Corp., 1977
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[Arlin]

Like rockguy said, inconctext is the way to go here if you are not using the hole series.

You can do this by either creating a skeleton sketch in the assembly and then edit each part incontext, relating the part sketches to the assembly skeleton sketch...
or
Create your cut in one of your parts, open the assembly and edit each part incontext and relate the cuts to the cut of that first part.

 

[MattP]

Thanks to everyone for the help. By "editing each part in context" do you mean converting entities from the cut in the first part to create a sketch in the next part?

 

[rockguy]

Yes. If you use the assembly sketch method you would convert the sketch entities from the assembly sketch.

 

[sloth4z]

This might help, probably not.

Sometimes it is easier to make an assembly level extrusion so everything fits perfectly. I don't know how to make those extrusions defined in the part so I just make a configuration with everything hidden except the part I need. I have to do this for each part with the extrusion. Than I can put the assembly in a drawing as if it was just the part.

 

[MattP]

That might actually help. You still wouldn't be able to see the extruded cuts in the part but you would in the drawing of the assembly which is just a drawing of the only visible part. The drawing is what I am after anyways, really.

Thanks,
Matt

 

[SBaugh]

Sometimes it is easier to make an assembly level extrusion so everything fits perfectly.

You can't make extrusions in an assembly... only cut extrusions.

(In your post) It sounds like your doing waaay to much work to accomplish this.

All you have to do is edit the part and the assembly stage then convert and enitity or create a new sketch derive it off other geometry in the assembly (other parts, planes or assembly planes, etc...). If your other components are not pickable (transperent., etc...) all that is, is a setting in Tool\Options - You will have to edit each part but you can use the previous part feature or sketch, etc...

Regards,



Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[JBN]

Can you not just create your feature patterned in the parent part and then in assembly create the mating patterns by using the "derived pattern" option? This gaurantees that the mating parts always have the same pattern, but you must decide on which part is going to be the parent and most desireable to be used as your "datum" part.

 

[sloth4z]

Oops, I meant cut extrusions. I know there are easier ways to do it, it's just sometimes people want things to be certain way and don't mind doing a little extra work to make it do what you want, the way you want it. This way might be easier if you had an angled cut. Otherwise you would have to define a parallel plane and then mate the extruded cut's sketch dependant on the parent sketch. And then if you did all the work expecting a feature that doesn't exist a work-around like this might be beneficial instead of going back and doing it proper.

 

[JNR]

I guess the brief answer to all this is to understand the fucntions.

Assembly features are something actually created at the assembly stage. So is it something you would, say, drill through all the parts in the assembly on the real thing?

You have to look at it as mimicking the real world.

If you are going to manufacture the features on the detail parts before they are assembled, them you want to design the individual parts to match each other. (As opposed to match drill them after assembly.) That is where editing the parts in the context of the assembly comes in. You are editing the individual part (not the assembly) but referencing features of other parts as they correlate to each other in the assembly. That way one part still changes the other.

From there all the tricks above should fall into place.

Be naughty - save Santa a trip.

 

[SBaugh]

The original question How do you bring assembly features (i.e. extruded cut thru multiple parts)into a part drawing? Or...how do you bring those features back to the part file? Is it possible?

If you want to make multiple cuts through several parts then you I would do as Madmango first suggested "Hole Series" You can make a holes series that reflects back to the parts at the assembly. Otherwise I would probably use multiple in-contexted features.

flyingblue -

http://www.scottjbaugh.com/Design_Portfolio/SW Models.htm

- Check out Example of In-contexting

Regards,


Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[downeyt]

To accomplish this feature in multiple parts, I would tile the windows and drag the cut extrude feature from one part to the next. The trick in doing this is keeping the feature self contained. Minimize references to the original part as much and possible.