In Solid Edge Frame Design Part 1, I introduced the Frame design tools and basic creation functionality. In this part I want to look over a bit of the software’s end treatment strategies. Also, I am trying to do these reviews in a somewhat conversational manner. Like I was talking through a video. I’m starting to think just creating videos would be easier. My team is cheering in the background. In any case, let me know what you think, please.
The whole deal with frame grouping is that the options for end treatments, among others, are fixed to the group. Each member in the group is sharing instructions. Such instructions can be tuned to individual nodes, however all members tied to that node are affected. If however, the intersecting member (in our scenario, the third frame member) is assigned to another group, then it can operate based on completely different instructions.
I have found a certain application of strategy pays off here. The best way to think of it is in terms of plane, and common behavior. In the case where my upper rectangle needs to rotate with the top skin, having them in one group made applying the rotation instructions very easy. Solid Edge seemed to know precisely what orientation was needed to rotate all members properly. The keys here were one group made up frame members that share a common plane.
Working the End Treatment
After fighting end treatments in Solid Edge Frame Design for awhile, I went to the help section. I wanted some insight into a few of the options. Like I have said before, Solid Edge is a great tool, but you really need some training to get the big ROI quickly.
I found a couple of things that I think you really should know. Miters are for two elements only. Not three, not four, but two. So if you have a intersection of three elements, automation is limited. Two out of three ain’t bad, unless you’re trying to build a frame weldment. That said, I would not want a full, three-way miter on this joint. The jigging and fit would be a complete bitch.
Let’s say you have a three-way intersection. If you want to do something clever with the third intersecting element, you can put it into a separate group. A rectangular arrangement of four elements that will be mitered together, like a base aligned to a single plane, can be picked at the same time. This will create a separate group for that base.
Changes seem to update through the entire group rather well, with clean automated end treatments. If you had the third, odd-ball element in the group, then the system would constantly try to fight the miter into the third element, and it would never work. Remember, the end treatments apply to the entire group, at the node selected. So pull the odd-ball out.
Adding New Members to an Existing Group
I started testing the corner treatments with 3 members, joined at the same node. I wanted to complete the frame base, by adding two more members to the existing group. It was really easy. Simply pick the group, then the selection button.
Next Solid Edge will ask you to pick the sketch elements to add.
After completing, the additional frame elements are created, in the group, and the end treatments are automated.
Let’s continue this scenario for a bit. You have four frame members built onto the base group.
You can now create the odd-ball frame member in a new group, with its own end treatment configuration. In my scenario, I want to fit the frame member completely to the joint. Why? Maybe it’s supposed to be pretty? In the options button I mentioned in part 1, there is an option for coping. When selected, along with the end treatment radio button, the frame member is automatically cut around the the joint. Friggin’ brilliant! After selecting this option, I rotated the base frame members longitudinally by 20 degrees. The coping updated without a hesitation (Figure 1).
Extend/Trim the Frame
On the other hand, there is definitely one part of this tool-set I do not like: The Extend/Trim workflow. Pick the member that you want to trim or extend. Next pick the end treatment button. Notice here that the dialog adds a check mark for accepting a selection. Solid Edge will automatically select both nodes of the frame member (the green ball at both ends). If you only want the instruction applied to a specific end, deselect the other. Next pick the green check-mark.
Solid Edge Frame Design interface and functionality will default to Extend/Trim. The command immediately prompts the user to pick the body, plane, or face to extend to. Notice there that those terms are singular. That is because only a single face is accepted. You can only perform the treatment for a single plane. If one trim has already been applied, a second one will override the first. Well isn’t that just ducky?!
Shouldn’t we be able to select multiple planes in this type of joint? YES!
I tried in addition to have it intersect the bodies of the frame members. It would only allow selection of a single body, and even then it did not extend well.
What can you do about this? Choose wisely. Personally, I’d add the coping option in the design, and whack off what was unnecessary during manufacture. In this way, you’d at least get the angles you needed to make the fit where you need it.
Solid Edge Frame Design has some really nice coping and fit capabilities. So far I find them to be responsive and pretty slick. Then again, there is the Extend/Trim functionality, or the lack thereof. It works fine if you are bringing the upper frame member down to a flat plane. If you have something a bit off, say like a 20 degree angle in your base (which I did in my design), then you have to work around it.
As a footnote, I went back in and created the 3-way joint in a single group. I tried adding coping to it, but no joy. The option is for joints that are NOT mitered. Hence the need to miter in one group, and cope in the second.
I still like these Frame design tools. I am just not ready, yet, to state that they are on par with the rest of ST10’s great features. A little more investigation is in order.
What will we review next time? Hmmm. Let’s explore monkeying with cross sections a bit in Part 3.