library features not behaving 3

[roadapple]

I am trying to use my library features, which are API 6A flanges. They will typically insert with no problems as long as I do not deviate from the orientation from which they are created. However, if I want to use a flange on each end of a part, then one side will work and the other side will return an error message that states: Unable to create library feature with selected references.

The funny thing is that all the geometry is in place and correct when this message appears. Once I click “OK” the geometry disappears – I and the placement routine starts over. I have forever wrestled with these problems since we switched to Solidworks from Pro-e.

Does anyone have any suggestions?

Roadapple

 

[EEnd]

I ran into a similar problem when I tried making library features. My library features were located off from some datum planes. The program did not like it when I selected planes that resulted in a different orientation. I think it was not able to handle different combinations of red and green sides of the datum planes, and there was no option to choose between them, (as there was in ProE when I used it last). After fiddling with them for a while, I gave up with the hope that they would work better in later versions.

Eric

 

[roadapple]

Playing with these I have noticed that chamfers will cause hick-ups. After I posted this I went back and deleted the chamfers from my Library part and re-inserted it - no problem.

It will just have to be a rule not to include the chamfers on the library part - they are easy enough to add but simple enough that I wish this wasn't a problem for Solidworks.

roadapple

 

[CorBlimeyLimey]

roadapple ... I have used fillets and chamfers on Library Features and have not had the problem you describe. I do not use LFs that much though, so my experience is limited.

EEnd ... Maybe LFs prefer to use the actual geometry they are being attached to, rather than ref' planes.

Can you both post a sample of a problem feature for analysis?
You may need to zip the parent file also.

 

[mncad]

We use LF's all the time. In fact every part file will normally have at least 2 LF's inserted. It took me awhile of using them to figure out the best way for everything to work. We have alot of LF's with both fillets and chamfers in them. Roadapple, are these API ring grooves that you are trying to insert? Like CBL said, a picture or file would be helpful.

mncad

 

[mncad]

Something I forgot in my first post. When doing LF's, create the base, which is just a generic solid to either make cuts on or add to in order to create the LF. For the next feature you create do not use a fully defined sketch. You will want to eliminate all Horizontal & Vertical references. Also, try to make everything in the sketch relate to itself, have as few references to the origin, the base or the 3 planes as possible, the less the better. After creating the first feature that will be in your library feature you will want to show the sketch, and then relate all future sketches back to the first sketch, not to the origin or to the planes. Also, you don't want to use a temporary axis for patterns and such, you will need to create an axis for something like that.

mncad

 

[roadapple]

How can i post either the image or the file?
roadapple

 

[CorBlimeyLimey]

faq559-1100
faq559-1177

 

[EEnd]

Here is the simplest example that I could come up with which exhibits the problem that I run into. The library feature has a single sketch which has 2 lines. One line is set collinear to the Right plane and the other is perpendicular to the first line. It works fine if when I place the library feature I select the Right plane in the base part. However if I select the Front plane, which I feel should result in everything being rotated 90 degrees, the inserted library feature cannot be resolved.

home.comcast.net/~ewetemp/SolidWorks/LibFeatureTest.zip

Eric

 

[roadapple]

Here is the problem I was trying to describe - the chamfer on the OD is what was keeping my LF from going into the part.

http://img525.imageshack.us/img525/9378/6bxflange1to3.gif

I am including both links as this "linkage" is new to me.

roadapple

 

[CorBlimeyLimey]

The base part was empty!

 

[mncad]

EEnd,

I looked at your files and have a couple of suggestions to try. First, delete all of the relations in your sketch except for the perpendicular between the 2 lines. Put a point on the line that you had colinear to the right plane, this point is what you will constrain to the origin (or whatever point you want) when you insert the library feature. Now when you insert the library feature it will only ask for a placement plane, under that will be a button that says "Edit Sketch". Pick this button and then the sketch of the first feature in the library feature will be opened for you. Then pick the point and the origin and make them coincident, then you can either pick the line and one of the planes and make parallel or you could even dimension at whatever angle you want. Hope this makes sense.

mncad

 

[CorBlimeyLimey]

Library features usually consist of features added to a base feature, but not the base feature itself. Because you cannot have two base features in a single part, you cannot insert a library feature that includes a base feature into a part that already has a base feature. However, you can create a library feature that includes the base feature and insert it in an empty part.

If you are trying to add the LF to an empty part, you are trying to create two base features and as explained above that is not allowed.

I created a rectangular block in the your base_part and was able to add the LF (correctly orientated) to opposite faces without a problem.

 

[roadapple]

http://www.mooload.com/new/file.php?file=file01/050707/1183648013/3-1_16+15K+STUD.SLDLFP&s=t

Can someone look at this LF?

If you start with a simple part - 14" OD and 14" long - it will insert in 2 directions. But if you extrude the base part in the other direction (90 degrees) it will not work.

For example - if you create a part with 2 cylinders 90 degrees apart 14 OD and 16 inches long - it will only go in on one cylinder that the LF likes.

roadapple

 

[mncad]

Roadapple,

I took a look at your LF and made some changes.

http://www.mooload.com/new/file.php?file=file01/050707/1183653810/3-1_16+15K+STUD.SLDLFP&s=t

I removed all of the axis that you created. I eliminated all of the horizontal & vertical relations in all of the sketches and related them back to the 2 lines in your sketch3. I also eliminated the cirpattern you had for the tapped holes and put the pattern into the holewizard sketch. Now when you insert the LF pick the face of the part that you want it on, the LF window will then show the "Edit Sketch" box, pick that. It will open the sketch3 of the library feature that is being inserted. Pick the circle in that sketch and make it concentric with your 14" diameter, then pick either of the lines and make one of the horizontal or vertical whichever you want. Let me know if that works for you.

mncad

 

[roadapple]

mncad - thanks for everything you are doing. But I am unable to read the file.

I am using SW 2007 SP2.2 - for whatever reason I am unable to open or insert the file.

Do you have a suggestion as to why this might be?

roadapple

 

[mncad]

roadapple,

I'm not sure, I'm using 2007 sp2.1. What kind of error is it giving you? I uploaded the file again. Try that once.

http://www.mooload.com/new/file.php?file=file01/050707/1183662407/3-1_16+15K+STUD.SLDLFP&s=t

mncad

 

[roadapple]

If I try to open it straight up - Error message is:

Seek failed on C:\address to saved file

If I try to insert it - it just doesn't do anything. Or if I open it from my SW library directory it doesn't do anything or return an error message.

I downloaded it twice - same result each time. I will try the new file now.

roadapple

 

[roadapple]

mncad - working now - thanks. Reviewing the modeling logic for other flange sizes.

roadapple

 

[CorBlimeyLimey]

Both LFs work fine for me with SW07-SP4.