I am a Creo Elements/Direct 18.1 user who is currently in the process of switching over to Solid Edge, and I'm very interested in the ability of the synchronous part environment to replicate a lot of the direct modeling capabilites I'm used to in Creo.
One thing that has been very useful in creo when modeling a part is the ability to cut by dimensioning the material remaining after the cut, so that I can quickly reach my design intent/goal without having to do the math to find out how much material to take away. Below is an example screenshot from Creo:
In this example, I have a solid of given length and I know that after I create the void, I want the bottom wall thickness to be 3", so I simply click workplane with the square profile on the top surface, then reposition the red cone to the bottom surface in order to measure the cut from there.
When I try to replicate this in Solid Edge, it does not work as expected. Below is a screenshot:
As can be seen, when I reposition the steering wheel to the bottom surface after initiating the extrude cut, and then pull down on the arrow, an error occurs and no cut takes place. If however I pull on the up arrow, it will start cutting FROM the bottom surface, even though my profile is on the opposite end of the part. I simply want it to cut from the surface with the profile, while measureing from the bottom surface.
Please advise on if it is possible to do what I am attempting in Solid Edge and how best to approach this problem? Thanks.
It is rather simple. Place your cutout depth by some arbitrary distance and then place a dimension from the bottom of the part to the bottom of the cutout and type in the correct value.
Thanks for your response, Grundey.
I was actually aware that I could do that, I just wondered if it was possible to achieve that result directly within the extrude command. It's not a big deal, really. I do know that when performing an extrude add to a part, you can add to the part in the manner I described in the post, by repositioning the steering wheel and inputing the new desired overall part length. Apparently cutting just doesn't have that capability yet. It would be nice to see in ST7, but again not really a big deal at the end of the day.
You can do this with a thin wall, but it becomes a proceedural feature, after making the thinwall feature click on the face that you want to make thicker and then click on the thickness dimension.
A little dialog pops up where you choose "Edit selected faces only" and enter your new thickness. Of course this is not synchronous, but halfway between synch and ordered.
Another way to do it is to make an synch cutout like you started to do to some arbitrary depth. Now click on the face you want to move. Set the offset like this: Hold down the shift key and click on the steering wheel arrow and move it in the direction of the new thickness and enter the dimension in the box, hit "tab" to set it and left click the direction you want the offset to be. Now click the arrow without the shift key and click on a point you want the face offset from such as any corner at the bottom of the box. If this doesn't make any sense I can try to make a video.
It seems like you should be able to offset the arrow after you select the cut region without going through the intermediate step of re-selecting the face, but I can't make that work. Maybe this should be an enhancement?
I don't suggest to look for same steps in SE what you already know in Creo/Direct.
Ken and lking give some solutions on Solid Edge's language.
Here are some others (other ways same result):