Rotate All when not in sketch mode?

[Talayoe]

Hello all,

Likely a simple question; I have completed a part and because I am new, drew it a certain way to make my life easier. Now that the part is complete I would like to rotate the entire part (but not create a new solid) by 45 deg. I cannot seem to figure how to do this.

Thanks 🙂

[Lance127]

What do you mean rotate it 45 degs. Do you need it to look different in the dwg\idw file or is it a matter of how it comes into an assembly?

[Talayoe]

Hi,

For this particular part there is not going to be an assembly, just an IPT and then an IDW. In the IDW I figured out how to custom view/rotate by angle to get the desired result (again, rotating the model by 45 degs from its center - being a round part).

But I suppose, by my currently limited view of software, I would have thought to rotate the actual model to get the required IDW base view instead of rotating the IDW into a custom view. I guess it works the way I have done it, but the question still remains wheather I can rotate a model (IPT - lets say from top view) by a given angle from the center point of the part...?

Thanks 🙂

[Lance127]

You can rotate to a set angle using the compass and view cube in the ipt.

Might be a better way but that is how I would do it.

[Talayoe]

I dont think that is quite what I am looking for. Rotating it using the viewcube it a temporary movement that will be reset when another view is selected. What I am looking for is a permenant movement of the entire part by said angle... Maybe its not possible because it isnt relevant the way the software looks at the models? Who knows.

Thanks for the input!

[Lance127]

After you rotate the view cube you can reset the "front" or "top" view to maintain it.

[Talayoe]

Hmmmm that is a good suggestion. Now maybe something with the viewcube i dont is how to rotate a specific angle. Is this possible?

[JDMather]

 I have no clue why you would really want to do this, but -

Click Move Body

change to rotation rather than translation and enter desired angle.

Attach your file here if you can't figure it out.

[Lance127]

Use the Compass the set the angle then reset the front view.

[SBix26]

Depending on how your part is modeled, you might be able to edit your first sketch, drop a constraint or two, then rotate your sketch geometry and re-constrain it in the position you want.  This is very likely to take more time than it's worth.  Another approach would be to just start again from scratch and model it the way you now know it should be.

Post your file here, someone may be willing to take a look.

[coreyparks]

What no one says for some reason is the best way is to model the part as you need to.  One that makes sense and makes it easy to work with as it sounds like you have.  Ignore the fact it's rotated 45 degs.  create the views as needed by rotating them during or after placement and project as needed.  Well will you look at that, seems you followed about the best way to do it from the start, good job!  For the most part the XYZ axis orientation can be ignored.  The only time I really pay attention is in assemblies so machines come into floor plan layouts standing up and not laying on their side, though even this is not a big problem to fix, that's what constraints were made for.

[Talayoe]

Its funny, I have started typing my response about 4 times now and get side tracked long enough that the authentication fails... silly system.

Anyways, the short is that my old habits from using other CAD/CAM programs previously HAD taught me that what I wanted to see on the paper was exactly how I MUST draw it. Not realizing until the end that this is not what I had done, naturally I figured I should turn it. Seem that is not quite the case here and to make point I suppose thinking about realize why it doesnt even really matter.

I appreciate all the input into this seemingly useless topic and hopefully over the next little while my -what may seem like basic or silly- questions will become more precise and useful.

I am glad this forum is here. Thanks all!

-R

BTW: the file is attached to look at if you want. The feature I wanted to rotate was so that the end resut made the Ø.595" thru hole to top and centered position. Thanks again!

[JDMather]

Here you go (see attached). 

[JDMather]

It also occurred to me that you might be doing a bit too much work - see attached.

[Talayoe]

Lol! Too much work i am sure! I honestly have no idea what i am doing. Had no formal training yet so i am just peicing things together.

Thanks for the file. I will have a look at it tomorrow at work

[JDMather · Accepted solution]

For someone who doesn't know what they are doing - you are doing better than about 90% of the files I see.

I think I only saw one sketch that wasn't constrained.

You might take a look at this document http://home.pct.edu/~jmather/skillsusa%20university.pdf

[Talayoe]

Thank you for that PDF. I will give it a good read through.

As for the constraint that wasnt setup, without having looked at the file I am going to bet it has to do with that hole that is on the OD of the part and the planes surrounding it. I got it to go for me, but had to muddle through it a bit.

As I said, I have actually been modeling (CAD only because I dont have the face or body for it otherwise 😜 ) for years designing jigs and fixtures, parts and other such things that go along with a Machinists career. But being that I wasnt using Autodesk products some of the ways about things will take some time to get used to, and also to wipe my memory of the old that I (currently) no longer need.

Thanks again for all the help, and I will haev a good look at that file here shortly! 🙂

-R

[JDMather]

---

@Talayoe wrote:

 ...I will have a good look at that file here shortly

---

Be sure to look at both the files I posted.
In first one I rotated your part.

In second file I redid it from scratch to show one (easier?) technique.

[Talayoe]

Hey JD,

I dont want to hassle you, not by any means, but I hope you dont mind if I ask you a couple of questions about that IPT you posted...your version of it.

I like how you constructed it, very simple and to the point, although there is some things there in that I do not understand. Btw if any of said questions are in that PDF you linked, just tell me to read that because I will not have time until I get home tonight to read that...likely.

1. Why do you change most of your lines to construction lines? I see them all over but do not understand why you would do this.

2. You created Sketch2 and then did ALL the BHC off that with the HOLE command. How is it that the Sketch2 is not consumed by the first HOLE command? I have tried something similar to this by creating multiple features and then I do one extrude or what have you and the sketch is consumed and the rest of the geom is unuseable.

3. The work plane creation is something we discussed in another thread. I see that you created the work plane in line with the hole on the OD without any geom towards the OD iteslf...Either I do not see or I missed something from that other post. Obviously you having seen my file, I created 2 planes to work my way around to the OD of the part, but yours seems so much simpler and I just want to understand said concept.

Again, dont want to hassle but you seem to be a high contributor and any help is greatly appreciated!

Thanks so much,

-Randy

[JDMather]

1.  I started out on the drawing board.  If it ain't an object line it's a construction line.  I know it isn't necessary - but I think it makes it more obvious.  I look at a LOT of files and things like this really speed up my analysis of the geometry.

2.  Any sketch can be shared by features - simply right click on the sketch and turn Visibility back on to use again.

Starting the Hole command it will automatically find all centerpoints - I simply Ctrl select the ones I don't want to use to unselect them.

3. See the angled line in Sketch2?

I simply clicked that line and the end of that line to create the workplane perpendicular to the line and at the end of the line.
Note:  If you change a dimension used to create a Workplane - you usually have to click the Rebuild lightning bolt icon to see the update in postion.