Sweep

[ausmods]

Hello all,

Im having a small bit of trouble and I cant seem to find a solution anywhere. Im modelling a thinner Xbox 360 case in inventor, and Ive got my curves that I want to sweep...

Ive attached the file to this post...

Basically, I want to be able to create a 2mm thick case using the curves in this file. The bottom loops will be the path, and the open curve will follow the path. I cant for the list of me figure out how to do it properly. Like I said, this case will resemble an Xbox 360, so you can get an idea of the curves there.

I can do all this in Autocad easily, but im still having a bit of trouble adapting to the strange new ways of inventor. Its bizzare when your used to Autocad.

Hopefully that all makes sense, like I said im still learning all of this :oops:

Thanks

[JD Mather]

I can do all this in Autocad easily, but im still having a bit of trouble adapting to the strange new ways of inventor. Its bizzare when your used to Autocad.


Geometry is geometry. The correct procedure to do a Sweep is no different in Inventor than it is in AutoCAD. The process is exactly the same.

Follow the evolution of this part through these threads
http://www.cadtutor.net/forum/showthread.php?t=33317

http://www.cadtutor.net/forum/showthread.php?t=33399

Including doing all suggested tutorials. When you have completed these I will walk you through your part just as I walked through the steps of creating the lofted hook.

[ausmods]

Geometry is geometry. The correct procedure to do a Sweep is no different in Inventor than it is in AutoCAD. The process is exactly the same.

Follow the evolution of this part through these threads
http://www.cadtutor.net/forum/showthread.php?t=33317

http://www.cadtutor.net/forum/showthread.php?t=33399

Including doing all suggested tutorials. When you have completed these I will walk you through your part just as I walked through the steps of creating the lofted hook.

Thanks for that, I was just having a look thru those threads and the tutorials, they look like theyll help a lot. Now all I have to do now is a full reinstall of inventor plus service packs... Vista has decided to not let inventor run at all (once again).

Its getting quite frustrating having to do a full reinstall every few weeks... Are there any known fixes? The main issue I have is when i start it, it gives an 'Inventor has stopped working' error.

[JD Mather]

Vista has decided to not let inventor run at all (once again).

Far more information is needed to diagnose the problem. I am running on Vista with no issues.

What version of Inventor?
What OS (32 bit or 64 bit)?
What graphics card/driver?
RAM and hard drive?

[shift1313]

i have the same issue with inventor 09 and im not sure why. It worked for 2 weeks then i got that error. Ive done a full wipe and reinstall and it still doesnt work. If you find the answer i would love to know:)

[ausmods]

Far more information is needed to diagnose the problem. I am running on Vista with no issues.

What version of Inventor?
What OS (32 bit or 64 bit)?
What graphics card/driver?
RAM and hard drive?

Inventor 2008, SP3
Vista 32Bit SP1, fully up to date
Nvidia 7900GT, version 181 graphics drivers
Athlon X2 4800+ processor
2GB DDR400 memory
200GB seagate SATA hard drive


Nothing out of the ordinary really...

[shift1313]

Inventor Pro 2009(dont know which SP cause i cant open it)
Vista Home Premium 64bit SP1
Intel Pentium Dual E2220 @ 2.4GHz
4.0GB ram(240pin ddr2 sdram)
NVIDIA GeForce 7100 / NVIDIA nForce 630i
500GB SATA 3G

[shift1313]

Well I got mine working again with some helpful internet info.

Per a post on another group some mentioned changing the appdata inventor file name. Once I did this Inventor opened up just fine. Im not sure for how long but i will keep an eye on it.

What I did was under my start menu did a search for 'appdata', opened the folder, go to Roaming/AutoDesk and there should be a folder called AutoDesk Inventor 2009. I renamed this folder by deleting the 2009 and Inventor opened fine. Now it did recreate this folder in the same directory so it would appear that its having trouble re-using this directory. This folder i think is used for temp data, undo, etc.

[shift1313]

so what is the trouble with the sweep? It sweeps just fine for me. I use your sketch curve as my path and set the orientation to parallel so my start/end are parallel planes.

[ausmods]

Yeah I did end up managing to make it sweep like that... The thing is that when I did it in autocad, the curve was 'rotated' appropriately as it went around the path, so that the middle of the case is the thinnest.

Lol, I'm not much good at explaining this.

Im after the same kind of curve as what you'd find on an xbox 360 case, where each part of the case is concave. Just have a look at an Xbox 360 case and you'll see what I mean (hopefully). Sorry for the dreadful explanation there.

I can post up a drawing or anything else if noone can make sense of my post... Or the autocad drawing I did.

Although, now I think about it, I might have swept each part of the case separately in autocad... Can each part of the case be swept in inventor, and then joined to form one whole piece? In autocad I had the path separated into 4 parts, the front and back cruve, and then the 2 straight lines, and then I did 4 separate sweeps...

BTW thanks for those tutorial links JD, they were a huge help. I also got inventor up and running after a full reinstall aswell.

[shift1313]

sorry but i dont have an xbox 360 but if you'd like to send me one id gladly study it for you.:)

As far as the shape you are looking for. if you need all 4 sides to concave then sweep is not the operation you want(and a sweep in any acad wouldnt give you that either). You will want a loft operation. I suggest you do this with a copy of your sketch at the end plane and rails at control points.

First I turned on the visibility of the xy plane in your drawing, then created a work plane offset from this by 276mm(the height of your curve). Sketch on that plane and used Project Geometry then Break link for all the lines of your "case" sketch.

Then i created two more work planes to draw my rails on(I only drew one rail and a reference center line, the mirrored it and projected it. This way all 4 are identical, but they dont have to be).

the yellow points on the drawing are work points. I made those for visibility. Your rails need to be coincident with your sketches(both of them) unlike the sweep operation where it could be anywhere. When sketching my rails i projected the geometry of one of the curves of the base sketch(the larger outside curve) and this brought a line(which i converted to reference) so i could create this coincident constraint.

All these things are important. I suggest you go through the tutorials and look at the inventor help file for Lofting with rails to get an understanding of the procedure since i didnt spell out everything here.

[shift1313]

here is an X for you

[ausmods]

Ahh brilliant, thats exactly what im after. Ill read up on lofting and give this a go. Ill report back when I have success.

Once I know how to do this, I can play with the curves to get the look of it right.

Thanks for that Matt, much appreciated.

[shift1313]

no problem. Since my curves were mirrored and projected i was able to change one curve and have the other change as well.

I would make sure you understand projected geometry, breaking links(if needed) the selection process for lofting etc. I dont know right off hand but im sure one of JDs tutorials walk you through this.

good luck

[ausmods]

OK, ive been doing a lot of reading and learning, which has been great... My knowledge has increased 10 fold... Its certainly a challenge to learn the new ways of inventor. Ive got a long, long (long) way to go, but im enjoying every minute of it.

Anyway, Im close to having this case right... But its not quite right at the moment..

The sides of the case, all the way around, should be convex. My drawing is convex on the left and right sides, but the front and back of the case have done something weird, I dont really know whats gone wrong... See the attached pics and my ipt file and youll get the idea.

I really wanted to refrain from asking more questions and do this myself, but this has me stuck...

[JD Mather]

Need a convex rail on each side to guide the loft.
Zip and attach what you have so far if you can't figure it out.
Nothing wrong with asking questions as long as you are putting in the effort.
Certainly don't waste time beating your head against the wall when there is a 2 minute explaination from someone with more experience.

[ausmods]

I zipped and attached what I have so far in my previous post... It all looks like what Shift1313 has in his attached pictures, but for whatever reason mine just didnt turn out quite the same...

The file I did attach hasnt had the loft done on it yet, I can attach a file with the loft done if need be...

[ausmods]

Success, I added another rail to the front and rear of the drawing, and I also re-did the rails so that they only bend in 2mm, instead of 5mm like the origional. That seems to have fixed the problem.

Thanks for the help guys :)

[JD Mather]

I didn't see your attachment before.

It looks like you are still doing way way too much work. Did you go through the tutorials in my signature?

[shift1313]

his attachment is in his first post JD but i dont think it will reflect what he has there.

What is too much work? All the planes he is adding? If his sketch was based in the correct place around the origin I can see him saving time and only creating 3 planes.

Ausmod, you can(should) use your origin and the origin planes for your base. If your first sketch was based in the xy plane and you had your origin and the x and y axis on you could draw a 1/4 of your drawing and mirror it about the x and y axis. then your XZ and YZ planes could be used for your guides or rails.

[JD Mather]

What is too much work?

In addition to using symmetry about the origin there are way too many points in the splines. Many people have the misconception that more points is better in a spline when in fact just the opposite is true. The best spline has only two points (of course that best case isn't always possible).

Search Google on Ed Eaton Curvy Stuff DiMonte Group tutorials for good treatment of this topic. The tutorials are written for SolidWorks but the geometric principles are the same for any CAD software.

[shift1313]

wouldnt a spline with two points be a line:)

I didnt notice any nodes on his splines. My screen shots had multiple points but i wasnt worried about the end result but speaking of which, can you add nodes to splines after creation in inventor? ive done this in ugs but never tried with IV.

[JD Mather]

wouldnt a spline with two points be a line.

Right click on that "line". You can do a lot to change the curvature (Inventor or SolidWorks).



...can you add nodes to splines after creation in inventor? ive done this in ugs but never tried with IV.

Yes (Inventor or SolidWorks). Mather's rule, RMB (Right Mouse Button) everything.

[ausmods]

Alright, heres a quick silly (and hopefully easily answered) question, I cant seem to find how to specify an exact offset distance in a sketch (eg, 2mm)... Nor does the cursor want to snap to the grid whilst im doing an offset... What am I missing? Or what setting do I have wrong?

Any ideas?

[JD Mather]

What am I missing? Or what ... do I ... wrong?

Any ideas?

You are trying to use Inventor like AutoCAD. The most efficient method to learn Inventor techniques is to get some professional training.
Distances are controlled by dimensions. Simply dimension your geometry.
http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

[shift1313]

Right click on that "line". You can do a lot to change the curvature (Inventor or SolidWorks).



I was just kidding around. I create two point splines and turn the curvature handles on.

Will inventor only do point driven curves or will it do a "best fit" bezier curve as well? I know 2010 seems to have a few more options when it comes to splines but I still dont see a "best fit" for fit method.