I would like to make several cuts in a sheet metal part after the part has been bent up (they are too close to where the bends are). Is there any way to exclude these cuts from the part's flat pattern? (Since they wouldn't exist at that time and I don't want the sheet blank cut out to have them)
Thanks
HI
Just suppress the cuts you dont want in your blank before you save as DXF. Remember to unsupress them though before you print the drawing.
Thats how I do it.
Thanks
Steve
Hey Otis,
You can try making a new configuration for your part with these hole suppressed. That way you have a configuration for both pre and post hole cut operation.
Ben
I like where you are going with this. My only concern is that if I have to change something it won't propagate through the configurations (like if I increased a flange size or something in the pre cut would that change trickle to the cut state). I am going to sniff around this option tho. Maybe a derived configuration would work?
Otis,
When changing dimensions, you can choose to make the change to all configurations or specific configurations. You can also have this new configuration maintain updated features not applied to it directly by adjusting the configuration options...
If you make configurations of a part the changes will be in the part where ever that feature exists. Thus if you have 2 configurations, one with holes and one without and yu change a flange size, it will change in both configurations. Of course that is as long as the flange isn't a child of the cut.
If the cuts are simply suppressed in the flat pattern there would be no problem either. The benefit with having two formed configurations is that you could have a before and after drawing showing as formed and then a view showing where to cut the holes.
does your flat pattern get saved as a DXF file to be sent to a laser or punch?
If so when you save a DXF, another screen comes up before it saves with a DXF preview of the part. On that screen there is an option to delete any entities you wish to delete. This DOES NOT affect the 3D model, just the DXF file. The down side to this is you have to click each entity (line) then click "Remove Entity" or use CTRL and click all of your entities then "Remove Entity". I use this feature quite often especially if i have chamfer around the edge of a flat part. The punch or laser operator has nothing to do with that and has to be machined; therefore I delete the chamfer lines.
Is this a new feature? I'm using SW 2015 and I don't have that screen coming up. It looks useful.
I am not sure. I was out of the Solidworks "game" for a while. I got back into it 2 years ago (2016). It has given me that option ever since i have gotten back into SW with this company.
Create you sheet metal part.
Make a drawing of that part.
Insert the flat pattern of the part (this will create a derived configuration named xxxxSM-FLAT_PATTERN)
Go back into your part. Activate the flat pattern configuration. Suppress the cuts you don't want cut.
This will give you a formed part with all of your features and a flat pattern with only the features you want cut.
How do you do that across multiple configurations? It only created one derived configuration for me. I'd like it to create two more for the two separate length configurations of this part, but it only did it for one of them.
It has:
9 Inch
52 Inch
117 Inch
9 InchSM-FLAT-PATTERN
Should I just type in the 52 and 117 derived configurations and then suppress the miter cut feature?
I should also note that doing what you suggested does not suppress the miter cut feature in the model when the part is flattened. However, it does suppress them on the flat pattern on a drawing.
Delete your flat pattern configurations..... Create a drawing --> insert the length you want (52"). Then you can change it to flat pattern in the drawing. This will create the derived configuration.
You need to co into each flat pattern configuration in the model and unsuppress the miter cut. You should be able to do this through a design table as well to save time.
I see so I have to have placed the flat pattern view in a drawing beforehand, and then it creates the derived configuration. Kind of a PITA if you ask me,
Thanks!
If a PITA is the program creating a configuration and suppressing a feature all while I'm creating a drawing view I need, I'll take the PITA way over the way it used to be.
Hey Otis,
You can try making a new configuration for your part with these hole suppressed. That way you have a configuration for both pre and post hole cut operation.
Ben