Design Xpress - Draft Angles Over 59 Deg.

[nlh]

I was wondering what I can't perform an extrude cut or extrude boss with a sidewall draft angle of over 59 degrees? I have a part I'm trying to model that has a tapered pocket .2 deep with a wall angle of 65 degrees. Is there possibly a setting that is not right? Does anyone else have this problem?

Thanks,
Nate

[tobyaxis]

Tjones might be able to answer this for you. Send him a PM with a Link to this Thread.

He is very good with Alibre. He helped me to create this in 8 minutes with the Free Version 9.2.

[tjones]

I am not sure why but Alibre restricts the angle to under 60 degrees (59.99999 will work).

But there is another way. Extrude with no taper then use the draft surface feature. Feature>Draft and then put the angle as required.

[nlh]

Wow Toby! Nice part. Is there any sort of tutorial for doing that? Did you use Xpress for that?

I've attatched the drawing file that I've been working with. The pocket needs to be on the largest face and extend inward .22" with65 degree walls from the outside edges(should be a sharp edge when done) , then need to put .375 fillets in all inside corners.

Nate

[tjones]

He did use Express for that. And can export to a stp file for loading into Bobcad for machining as well.

No there was no tutorial just for that (other than step by step phone call).

Not bad for a free program!

[tjones]

I was able to easily do the part the way you want using the loft cut.

Create a plane .22 (depth you wish to cut) from the top plane.

Now you will need two sketches for the loft cut feature.
a) create sketch on top surface and use the 'project to sketch' to get the outside edges to be in the sketch as shown
b) create a new sketch on the .22 plane and use the offset to create the lines at the correct distance for the angle (.4718")
c)create a loft cut using these two sketches for the cut.


Now add the fillet!

[nlh]

Thanks TJones,

I'm still learing but so far I really love this free version of Alibre. Heck, can't beat the price even if I do upgrade to Xpress Plus!

I'll follow your steps to make sure I get it down correctly. I wasn't sure what the loft command did. I will be exporting this file to BCC2007 for machining.

Nate

[nlh]

Ok, I seem to be doing something wrong although not sure what. When I try to loft cut my 2 sketches I get an error

"CLOSED_EDGE: Closed edge in multi-edge wire"

I made an plane offset .22 from the front face. The projected the top face sketch to the new plane, offest by .4718, then deleted the outer portion of sketch, the selected the top face and projected sketch to that one. The selected loft cut, held shift key down and selected both the top and bottom sketches, clicked ok and get the above error. What am I doing wrong?

Thanks

[tjones]

Most likely you have the offset sketch wrong.

The trouble may be that the originals need changed to reference figures (you have two sets of lines in the one sketch).

To change the original outside lines to reference figures:

1)right click the sketch and select edit
2)right click each of the projected lines (not the offset ones in the sketch) and select 'convert to reference figure'


BTW: When you 'project to sketch' a set of lines that will not be used in the feature (reference only) you can check the box in the pojection window to do this automatically.

[tjones]

I guess I should have fully read your post. I didn't see that you deleted the original projected lines.

Maybe you should check each sketch for errors.

Sketch>analyze check all the boxes and click Analyze. This will tell you if things like untrimmed lines or open contours exist in the sketch.


Also make sure the offset plane is .22 below the top and not above it.

[nlh]

Thanks Tjones,

Turns out the hole in the center of both sketches was causing the problem. I was deleting the one on the offset plane but forgot about the one on the top face. After getting rid of those it worked perfectly!

[tjones]

I understand then.

When you did the 'project to sketch' it defaulted to the face. For future reference remember two things.

First is that if you are only using the edges for reference use you can keep it parametrically linked to the form by checking the 'maintain association to source' and you can default the projected lines to a reference figure by checking that option.

Second is that you can remove the defaulted surface and select the individual edges that you wish to project.