Working in the 2D model sheet of free SE2D I am finding it impossible to add more driving dimensions to lines that are newly added to an existing body of inter-connected lines. This body of lines was drawn a while ago and carries numerous driving dimensions already. If I add a single line that is not at all connected and then add a dimension between that new line and part of the existing body of lines (using either “Smart Dimension” or “Distance between”), I only get driven dimensions and these cannot be switched to driving by clicking on the padlock button in the small window that shows when you click on the dimension.
I do have the maintain relationships button activated.
If I draw a line near a separate but similarly complex body of lines in the same model sheet I do get driving dimensions - as expected. Also, if I open an earlier version of the same SE draft document I can add lines and get driving dimensions on the same body of lines that is now giving the problem. So it seems to me that the problem is with something I’ve done to the body of existing lines rather than the current settings for adding dimensions.
This problem occurred once before and I had to delete much of the work and re-draw it.
I would be most grateful for any advice on how to rectify or avoid the problem.
Another (possibly related issue ??) is that from time to time several of the existing dimensions suddenly start displaying in a colour that indicates they are “Error dimensions”. I can’t find out exactly what this means but I assume it indicates there is some inconsistency in the dimension. However, I find that if I drag the text of one of these apparent “error dimensions” small distances with the mouse then the colour reverts to normal (black in my case). Once this colour change starts happening for a body of lines it seems to re-occur from time to time.
It may be a coincidence, but both these problems have appeared since I started using the Variables Table to define variables and then equate the driving dimensions in the model to these variables.
Can you send the draft files to me. I will take a look. I need the one before the error dimensions and the one after. You can email them directly to me instead of posting to the news group.
I'll try to explain what may be happening. Solid Edge uses DCM solver for constraining geometry. Constraints on geometry include everything that holds the geometry into a specific condition. These include dimensions and constraints such as horizontal/vertical, connect, concentric, colinear, etc. All geometry that is connected through these constraints are passed into the solver collectively to be solved. Every time you make a change to the constrained geometry, a solve takes place. When a dimension goes sick, it is because a condition has occurred wher the solve fails. I cannot simply say it is because of this or that because every failure is different.
You will have more success if you try to simplify the constraint system. This can be done in a number of ways. If you use duplicate geometry you will be better off using blocks. Geometry within a block is constrained to geometry within the block. But, the block solves as a single entity when placed on your drawing. This reduces the number of constraints that are being put into the solver.
You can also create Ridged Sets of geometry. This allows a set of geometry to be collected together and again solvew as a sintle unit. this again reduces the constraints in the solver.
Thanks for that explanation - I do use blocks but, thanks to your reply, I now understand more about why they are useful - i.e. in addition to their basic convenience. Am I right in thinking I should use them rather then replicated groups?
Actually I dicovered by chance that selecting the whole block of problematic geometry (with all it's dimensions and relationships) and dragging it across the sheet a small way cleared whatever it was that was causing the problem and I can now add more new lines and driving dimensions. Does this make any sense? Your message gives me a degree of insight into what goes on when using the software and I'm wondering if the movement triggered some sort of more radical re-calculation of the geometry.
I'd be happy to send the files to you but since the problem is rectified (at least for the time being) maybe you have more important things to do than study my amateurish documents. Please let me know if you want them.
Could you please explain what you mean by "Ridged sets of geometry"? This does not see to be listed in 2D drafting help. I shall endeavour to follow your advice - although I am sure that compared to many peoples applications my drawings are not all that complex.
I am glad you resolved your issue. I can see where modifying a large set of geometry could resolve the issue, but I will not go into the details of why.
There is a command in hte relate command group called Rigid Set. This is what I am refering to. Place a rectangle. Run the Rigid Set command and fence select the lines of the rectangle. Click the green check to accept the rigid set. You will see constraints added to the lines that look like littlt diamonds. This says that the lines belong to a rigid set. To delete the set, click on one of the diamonds and delete. While the lines are in a set, play with dragging the lines and notice that they all move together. This reduces the scope of what is seen from outside the set. Even though the lines have connect and horizontal/vertical constraints, anything outside the set does not know that. All anything sees outside the set is the set itself. This can greatly reduce solving of the 2D geometry constraint system.