library features not behaving
library features not behaving
(OP)
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
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






RE: library features not behaving
Eric
RE: library features not behaving
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
RE: library features not behaving
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.
RE: library features not behaving
mncad
RE: library features not behaving
mncad
RE: library features not behaving
roadapple
RE: library features not behaving
FAQ559-1177: How Do I Make Files Available For Download? ... No Emails Required
RE: library features not behaving
home.comcast.net/~ewetemp/SolidWorks/LibFeatureTest.zip
Eric
RE: library features not behaving
http://
I am including both links as this "linkage" is new to me.
roadapple
RE: library features not behaving
RE: library features not behaving
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
RE: library features not behaving
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.
RE: library features not behaving
http:/
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
RE: library features not behaving
I took a look at your LF and made some changes.
http:/
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
RE: library features not behaving
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
RE: library features not behaving
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:/
mncad
RE: library features not behaving
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
RE: library features not behaving
roadapple
RE: library features not behaving
RE: library features not behaving
CBL
The base part was intentionally empty as I was going for as simple of an example that I could reproduce the behavior in. As the library feature is just a sketch, I do not think that it is an issue of multiple base features. The behavior that I see is when I insert the library feature with the placement plane as Top and the Right plane selected as the Right reference, the library feature inserts ok. When I insert it with the placement plane as Top and the Front plane selected as the Right reference, the library feature inserts, but the resulting sketch gets flagged with the warning triangle and is considered not updatable. Does it not behave this way for you?
mncad
I removed the locating constraints and used the edit sketch button to specify the location and was able to achieve the desired behavior. This is conceptually different than how I was trying to use the library feature. I was trying to push the method of locating the feature into the feature definition. Your way leaves locating until the placement step. In addition to providing more flexibility in the placement of the features it has the added bonus of working. I will try it that way in the future. Thank you.
Eric