Sweep-cut with a solid body

[redbullah]

Hello, i used to use Solidwork's sweep-cut with a solid body feature but i can't find it in Inventor now. Any suggestions?

Procedure:

In part file;

Create a second solid body (must be axis-symetric, like revolved feature),

Create a path that intersects with the solid (can be a line or a curve),

Sweep the solid along the path with cut command.

I need this where the sweep-cut with a profile is not enough, to get surfaces obtainable by milling on a cylindirical body on a helical path.

[BMiller63]

There is a sweep cut shown toward the end of this video (if you can view youtube):

http://www.youtube.com/watch?v=Z5lf4sGAQfc

another couple here:

http://www.youtube.com/watch?v=aE6IiqRLR5U

http://www.youtube.com/watch?v=QmK45L23pu8

[redbullah]

Thanks for your response but in the videos sweep-cut is made by sketch profiles. I need a solid body instead of sketch profiles, or some way similiar to it.

[BMiller63]

ahh, I think you're looking for the Combine command then, you can use it to cut one solid from another, provided of course that you have 2 solids.

Here's a video showing one part being cut from the other using the combine tool (toward the end at about 4:00):

http://www.youtube.com/watch?v=11dyV4InbmI

[redbullah]

Not really, let me explain it in a simple way: I want to sweep a solid body along a path, and this body to cut other solid bodies on it's way. Just like milling...

[redbullah]

Here is what I'm trying to tell: http://help.solidworks.com/2010/english/SolidWorks/sldworks/LegacyHelp/Sldworks/Features/HIDD_DVE_FE... http://www.youtube.com/watch?v=KdPptjqst6U&feature=related (after 5:00) I want to define a tool body to sweep-cut like this. I hope linking solidworks stuff is no problem. 🙂

[yannick3]

Hi

Just like milling...

I understand you correctly inventor can't do that.

but like milling, sweep path with 2d sketch is the same thing, but the only bug i've imagined in your design is that section is not symetric; for this purpose use two  2d sketch with the same path

[redbullah]

Inventor can't do that? I don't want to believe that... :'(

[JDMather]

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@redbullah wrote:

Inventor can't do that? I don't want to believe that... :'(

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Attach your ipt file here.

[BMiller63]

thanks for the swx links, I see what you're after.

no, Invenrtor can't do it that way, but you may be able to use a standard 2D sweep to get the results you're after.

or you may not.

if you search this forum for keywords such as "helix sweep" or "end mill sweep" etc you'll likely find many examples of past topics on this, and some example files that may (or may not) help.

Inventor needs to have this ability. So you might go to this link and request it. Although I'm sure that's been done in the past, it still helps (I hope).

http://usa.autodesk.com/adsk/servlet/index?siteID=123112&id=1109794

also, if you attach your file as JD mentioned I'm sure you'll get some help determining the best way to pull it off with the tools Inventor has.

[redbullah]

@ JDMather,

I made up an example here. In this part file, I want the "tool body" to sweep-cut along the "path". The surface that I want can NOT be done by 2D sketch profiles, I ensure you i tried lots of variations.

Thanks for your interest.

[JDMather]

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@redbullah wrote:

@ JDMather,

As you see, that answer does not solve my problem, so why should i accept it as a solution? I am sure there is some way Inventor can do it.

I made up an example here. In this part file, I want the "tool body" to sweep-cut along the "path". The surface that I want can NOT be done by 2D sketch profiles, I ensure you i tried lots of variations.

Thanks for your interest.

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As you should have seen redbullah the "Accept as Solution" is a canned tag-line that most of us have added to our signatures.

I have spent considerable time and effort on solutions to problems of this sort. (see http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%2011.pdf )

This method worked in Inventor or SolidWorks http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%2011%20Tutorial%2011.pdf before SWx added the functionality your referenced.

Since that time Inventor has also added functionality that might solve your problem more readily than the example in above tutorial - but it is not so easy to discover this new functionality.  When I get a chance I will see if it applies to your design intent.

[redbullah]

Yes, I figured it out after reading your other posts so i delete it.

Checked the pdf you sent, I appriciate your help but it still does not solve my problem. By the way, can you send the Cylindrical Cam.ipt file that named in the pdf?

No offense, I thank you so much 🙂

[JDMather]

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@redbullah wrote:

Checked the pdf you sent, I appriciate your help but it still does not solve my problem.

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The tutorial was a general-purpose solution written years ago with old technology.
When (if) I get a chance I will show the way solve your problem (if possible) today in 2011 (not readily obvious).
I do not see any reason it should be particularly difficult - but I haven't started on it yet.

[Doug_DuPont]

I needed to change your process a bit. I made a sketch perpendicular to your path first. When sketched your ballnose endmill on that sketch. When I Offsetsurface your OD. When  sweep under type I selected Path & Guide Surface and cut the path. When I made sketches on both ends of the path and revolve cut the ends.

I see you are using an older version of Inventor so I did not post my part.

Doug

[yannick3]

Hi

''I made sketches on both ends of the path and revolve cut the ends.''

If you create prameter named Dia_endmill and create edge fillet (on both sweep's  end) with Dia-endmill/2 radius you save some time and click

[redbullah]

dear Doug_DuPont,

that was the first method i tried to create semi-spheric ends, but no matter i create sketches at the ends and revolve-cut them, i've failed to get the absolute right tangency. but your method seems like a success. if it is inventor 2011, i can check it out in the office, can you send the .ipt file please? by the way your tool body profile's axis seems like parpendicular to part's axis and intersects with it, right? i need some angle for tool body's profile.

thanks for your efforts 🙂

[Doug_DuPont]

Here is your Part1 that I mofified.

We design and make a lot of cutting tools and if Inventor had the ability to sweep cut with a toolbody it would help us so much.

Maybe JD can look at it also and give us 2 cents also.

Remember to drag the EOP marker to the bottom of the browser.

[redbullah]

thanks for your reply. but i can't see the modified part in Inventor View 2011 x64. have you got any ideas? 

[Doug_DuPont]

Did you pull the end of part marker down in the browser?

Doug