vertical horizons Posted March 23, 2010 Share Posted March 23, 2010 I built a 2" 45° elbow. (See the zip file.) I have a problem attempting to use the CONSTRAINT command on this elbow. I can grip one opening of the elbow, but not the other. Therefore, I can constrain the elbow to one item on one side, but I can not constrain anything to the other opening of the elbow. I am using CONSTRAINT > INSERT. Any ideas as to why I can only grip one end? Q9405 Elbow 2 Inch 45.zip Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 23, 2010 Share Posted March 23, 2010 Your first sketch is placed at the origin but not constrained to the origin. Read this document http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf Workplanes 1 & 2 are duplicates of the XY Plane and therefore not needed. Sketch2 is not constrained - it could be used for the length so Sketch3 and Extrusion1 are not needed. Your sweep path arc is not constrained to the origin. The center is not horizontal to the origin. The radius is some really odd-ball number. I can walk you through this step-by-step, but you have to be willing to follow my steps exactly. Let me know. Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 24, 2010 Author Share Posted March 24, 2010 I can walk you through this step-by-step, but you have to be willing to follow my steps exactly.Let me know. I am always willing to learn. I appreciate all the help I can get. Just tell me what I need to do. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 24, 2010 Share Posted March 24, 2010 Start a new part file and create the sketch as shown. Attach the ipt file here. Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 25, 2010 Author Share Posted March 25, 2010 Here you go. Elbow.zip Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 25, 2010 Share Posted March 25, 2010 Your first sketch is placed at the origin but not constrained to the origin. You should not be able to drag the line anywhere on the screen. Read this document http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf Inventor will by default automatically place a coincident sketch constraint to the origin - so you have changed something on your machine that you should not have changed. Make sure your Application Options are set as suggested in the linked document. You could select Project Geometry and select the origin Center Point in the browser to fix your sketch. Then drag the left endpoint of the line away from the origin and then back to the origin. You should see a green Hard Snap indicator and the line should change color indicating that it is fully constrained. This is the most basic of basic techniques to be understood before you can continue in Inventor. If you can't get your sketches constrained you might as well go back to AutoCAD. Let me know when you have the line fully constrained. Also, in the upper right corner of your screen when in the sketch environment there are two icons, Constraint Inference and Constraint Persistence - make sure you have not toggle these off. You should never-ever use these two tools. They are not needed to be ever turned off (there are better methods to do what they do.) Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 25, 2010 Author Share Posted March 25, 2010 ...Inventor will by default automatically place a coincident sketch constraint to the origin...Let me know when you have the line fully constrained... I made the changes, as per your link. I then erased what I had created earlier, and redrew it. I do not know if I have drawn it correctly. When I checked "SHOW CONSTRAINTS", all I get is the "HORIZONTAL CONSTRAINT" symbol. ...make sure you have not toggle these off. ... Both of them are turned on. Quote Link to comment Share on other sites More sharing options...
shift1313 Posted March 25, 2010 Share Posted March 25, 2010 I made the changes, as per your link. I then erased what I had created earlier, and redrew it. I do not know if I have drawn it correctly. When I checked "SHOW CONSTRAINTS", all I get is the "HORIZONTAL CONSTRAINT" symbol. Both of them are turned on. One easy thing to do is grab the line and see if you can move it. You should have a coincident constraint icon so it is missing. You can manually place one between your line endpoint and the origin. I cant recall if 2009 let you use the origin without projecting it. Older versions did not and 2010 does. If it will not let you place a constraint with the origin, click on it in the model tree and use Project Geometry in your sketch. then place your coincident constraint with this projected point(will be a purpleish color) and your line end point. Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 25, 2010 Author Share Posted March 25, 2010 ...You should have a coincident constraint icon so it is missing... When I went to add the COINCIDENT constraint to my line, it said that there was already a coincident constraint in place. What's next? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 25, 2010 Share Posted March 25, 2010 What's next? Is it there or not? You have to know what Inventor is doing - no guessing. Did the line change color? Can you drag the endpoints of the line? If you can still drag the endpoints then I suggest you simply start over from scratch till you get this right. Set the Application Options as I suggested in pdf document. Sketch the line and it should automatically snap to the projected origin when you created it. Quote Link to comment Share on other sites More sharing options...
shift1313 Posted March 26, 2010 Share Posted March 26, 2010 VH, here are some screen shots. Start by drawing the line in the first one. this line doesnt snap to the origin, is not above the origin and is not horizontal. First add a coincident constraint with the origin point and the end point of the line. Next add a Horizontal constraint to the line. Next add a dimension to the line. Note: after you add the coincident and horizontal constraints the line will turn black, but it still needs a dimension to be fully defined. It turns black because its position is fixed and only its length can change. Before you add the dimension you can grab the "free" end of the line and pull it. The reason i am telling you to draw the line in such a manner is so no constraints are added and it lets you understand what you are adding. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 26, 2010 Share Posted March 26, 2010 Start by drawing the line in the first one. this line doesnt snap to the origin, is not above the origin and is not horizontal. I think you meant something like, "...is above the origin...". Quote Link to comment Share on other sites More sharing options...
shift1313 Posted March 26, 2010 Share Posted March 26, 2010 well i meant is not directly above so no vertical constraint would be added. but i guess yes it is above the origin Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 26, 2010 Author Share Posted March 26, 2010 ...First add a coincident constraint with the origin point and the end point of the line. Next add a Horizontal constraint to the line. Next add a dimension to the line... Note: after you add the coincident and horizontal constraints the line will turn black, but it still needs a dimension to be fully defined. It turns black because its position is fixed and only its length can change. Before you add the dimension you can grab the "free" end of the line and pull it. The reason i am telling you to draw the line in such a manner is so no constraints are added and it lets you understand what you are adding. That made it a lot clearer. (Great explanation.) I redrew the .ipt file. I can now see both the coincident & the horizontal constraint symbols. Elbow.zip Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 26, 2010 Share Posted March 26, 2010 Now that you have the line, sketch a circle with the center of the circle at the right endpoint of the line and the edge at the origin (left endpoint of the line). Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 26, 2010 Share Posted March 26, 2010 Then sketch a line from the center of the circle to about 45°. Add the 45° dimension. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 26, 2010 Share Posted March 26, 2010 Trim the circle (shortcut hit x on the keyboard) by selecting the part of the arc to remove as shown. Change the two lines to construction linetype (select the lines and then the icon to change to construction linetype is in upper right corner of screen). Attach your progress here. Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 26, 2010 Author Share Posted March 26, 2010 So far, so good. Elbow.zip Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 26, 2010 Share Posted March 26, 2010 So far, so good. Nope - you didn't get the lines changed to Construction linetype as I directed in previous response. You must follow my instructions precisely and if there is an instruction you don't understand - ask questions. Quote Link to comment Share on other sites More sharing options...
vertical horizons Posted March 26, 2010 Author Share Posted March 26, 2010 ...you didn't get the lines changed to Construction linetype... You're right. My mistake. Elbow 3.zip Quote Link to comment Share on other sites More sharing options...
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.