drawing question: inserting parts

[emc2673]

After finishing up my assembly I want to start to create drawing from some of the parts that I have built. Now I have gone trough the tutorials but they were unable to help me. First basic question when I built my assembly I constructed it in a top-down fashion so I continually inserted/component/parts into the assembly which in some cases I was able to mirror some parts, now when I go and try to create a drawing of those parts the mirrored "part" get inserted into the drawing as well... any hints as to get rid of the "extra entity" in my drawing?

last question since some of the parts that I created within the assy are at wierd profile angles such as 35 degrees is there any way in solidworks to rotate the part so that it lies at a "0" angle within the drawing?

Thanks again

 

[CorBlimeyLimey]

Cannot answer your "mirror" question yet, but for the "wierd profile angles" question, you will have to create a new view in the model which sets the part in the orientation you need to show in your drawing. Basically click on the face you want to show, then select the "Normal to" icon, then rotate the part using <Alt>+arrow keys to what you need, then set your new view using the View Orientation icon. When you call the part into a drawing you will be able to select the new view as the basis for any other views.

Read the Help > SolidWorks Help Topics > Index & type Orientation for further details.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[Arlin]

Can't help you with the first problem.

As for the second, orientation question:
You can also insert a "Relative View." This allows you to select a front and top face when placing the view.

The benefit of Relative Views over creating a new view in you component (as CorBlimeyLimey suggested) is that if the angle of the face changes, the Relative View will automatically reorient itself.

 

[TheTick]

The benefit of Relative Views over creating a new view in you component (as CorBlimeyLimey suggested) is that if the angle of the face changes, the Relative View will automatically reorient itself.

Did they finally fix this?

One caution about relative views:
When you insert a relative view into a drawing, there is no warning to inform you whether the view is set for projected or isometric dimensions. I had to write an addin to cover this after some users lost several hours redrafting.

Due to illness, the part of The Tick will be played by... The Tick.

http://www.EsoxRepublic.com

 

[CorBlimeyLimey]

Arlin
I must admit I had forgotten about the Relative View feature, but should point out that the preset view will also automatically reorient itself if the Normal to icon is used to set the model face for viewing.

It's just personal preference but I like to set the view orintation at the model creation stage, rather than at the drawing creation stage.

I have not used Relative View that much & have not had any problems with it, but TheTick obviously knows of some former problems. If those problems are now fixed, either method should work.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[ShaggyPE]

As far as the second quetion goes, you can also rotate your model to get the view that you want to be the front view and "update standard views". Do this by first hitting space bar to bring up the orientation control box. Rotate your model or use the normal to face option (I prefer the normal to face option). Now that the face you want as the front view is to the front, click on the word front in the view orientation box. Now click on the telescope looking icon in the oreintation box called update standard views. It will be as if you created the part on the front plane instead of in context to some other part. I use this technique all the time for parts that were created in context of an assembly.

 

[SBaugh]

As for the first question.

Are you saying that when you insert "Part A" into a drawing that within "Part A's" view that the mirror part appears with the same view window?

If you open up that part that you are making the drawing of. Make sure there isn't another body in the model? That's the first step to check out.

Regards,


Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

I think you are on the right track Scott.

emc2673
Can you explain how you created the mirrored part. It sounds like you have created a multibody part rather than a true mirrored individual part.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[emc2673]

I created the part "mirrored part" in the following fashion:

I inserted new part and created a name for it then selected a plane where I wanted the part to be placed. I than when about creatign the part as such and saved my finished part (within the assembly)since I did not want to create a rigth and left part I went to the mirror part icon and selected a mid plane (which to mirror from) then selected the part. clicked OK and voila the part was mirrored. Now some one told me about configurations? not to sure if the config. option will help in resolving this matter....

 

[CorBlimeyLimey]

emc2673
As SBaugh suggested, open the part you created the mirror from. If you see the mirrored part as well, then you have created a Multi-body Part ... which is not what you want.

You need to read the Help files to explain the correct procedure to create a separate mirrored part. Then insert it into your assembly.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.