I would make two part bodies to start one being the shaft or cone the second would be of one blade.
Once those two are modeled copy the blade two more times and rotate them around the shaft.
The blade could be built on a plane support that is at a given angle to the shaft say 45 degrees.
I agree. Multiple bodies would suit, but I'd use OPEN-bodies and surfaces for more complex geometry (Thicken or Close in Part Design at the end). Blade geometry, I suspect, would suit either Circular or Conic Sweep, or perhaps a Loft with pre-defined section profiles for better control. Consider using oversize surface(s), then Trimming to a profile.
Good luck.
I'm agree with V5Geek. For pre-defined section profiles try to use an example which is in the v5r11 on-line documentation (Idon't know if is available for other release). There is an excel file called PointsSplineLoftFromExcel which allow you to import points in an OpenBody. So you can create very easy the section profile of the propeller (of course, if you know the coordination points of the profile).
Puck - how do you copy the blade two more times around the shaft and rotate them? Circular array? Once you connect the blade to the shaft, its one part. Having same question on something similar...
Paul
>>puck (Aerospace) May 18, 2004
I would make two part bodies to start one being the shaft or cone the second would be of one blade.
Once those two are modeled copy the blade two more times and rotate them around the shaft.
The blade could be built on a plane support that is at a given angle to the shaft say 45 degrees.
911turbowing, you don't make the shaft and the blade into one part until you have created the other blades. Use Define in Work Object for the body with the blade in it. Perform a Circular Pattern with the body as the Object to Pattern. You can do a Complete Crown and put in the number of blades as the Instances. Use the Shaft as the Reference element or use some other element for the axis.
After you have made the other blades, THEN you add them to the body with the shaft.
OK, I understand sort of, but have more questions --
When you make the blade, if you attach it to the body (like extruding "up to next") it automatically becomes 1 with body. If I make the blade totally seperate from the body, then do like a copy/paste, the copy/paste doesnt seem to include all the fillets.
My next question is, does the circular pattern command allow chamfers/fillets to be copied? All I have been able to circular array is a pad or a hole. None of the chamfers go with it.
I dont know how to explain, maybe it would be easier if I could send or somehow post the file Im working on so one of you experts could see what Im doing. Ive obviously got something confused.
>Put the blade into a new PartBody within the Part Document. Do the same for the Hub.
Yes, you can pattern entire groups of features. You need to have them in a separate PartBody first.
Arggggh! By "new PartBody" I assume you mean insert a new body, right?
I did this, and i get the error message "the selected body isnt opered" whatever the f#ck that means. I thought I knew english pretty well, since its the only language IVe ever spoken. These error messages in Catia are making me doubt the english language.
When you try to use the Circular Pattern function, use the BODY as the object to pattern, not a specific feature like a pad or fillet or chamfer. This is important. If you make your propeller blade with Fillets or Chamfers on it, they will be included in the replication because they are part of the Body. You don't need to do a Copy/Paste operation. You make the object once, in its own Body and let the Circular Pattern replicate it as a pattern. Then, use the Boolean Add to join the propeller body to the shaft body.
