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Rip and Edge cuts?

K

kumaichi

New member
Hi Everyone,


I'm new to the sheetmetal world and looking for some help with rip and edge cuts. Below is a picture of a sheetmetal part I'm trying to make. It's the base for a machine so that I can catch coolant. It's tilted toward the front so I can direct the spent coolant to a reseviour. It's only the first part, I still need to make the flat areas around the base.


Anyway, I started with a solid model because I couldnt' figure out how to make the part in sheetmetal so I just converted the solid to sheetmetal which worked suprisingly well. Now I have my sheetmetal pan but I need to insert rip and edge cuts so I can flatten it out.


I tried creating an edge cut and by selecting one of the edges leading from the top down to the bottom, seemed pretty simple, select the edge I would like cut. I get the following error:


Could not construct feature geometry.


Since that didn't work, I thought I'd try a rip cut along the base flat piece at the edge I was trying to select. I go into sketcher, draw my line from corner to corner and I get the same error.


Could someone please help a newbie to create the cuts to flatten my sheetmetal part?


Thanks in advance,


Craig


The part file can be found here in case I did something wrong:


2005-10-02_182835_Base.zip


basesolid.jpg
 
The error is caused by the sheetmetalpart geometry, not an incorrect cutfeature. If you look at your model in wireframe, there should always be a white and a green side. On your model, there are areashaving green on both sides! This is the cause of your problems


Solve this by changing order of the smt conversion:


1. Create a shell feature (t=0.06) before going to SMT


2. Concert by defining driving surface


3. Create a SMT Conversionfeature that rips 4 edges


4. Sketch regular rip's in the 4 corners to open the geometry.


I have a completed model here i WF2 format if you are interrested.


/M
 
Caddie,


Thanks so much for troubleshooting the problem. I didn't even realize the part didn't have a green/white side.


I did your steps andthe Rip Edge cut worked beautifully. I am having trouble with the Regular Rips on the outside corners. Did you have to do anything special to get this cut to work?


If you could post the prt file that you have working I would really appreciate it. Maybe I can go through the steps and see how you did it on a completed piece. If you want, you can email the part to me and I can post to the forum.


Thanks again for all your help,


Craig


[email protected]
Edited by: kumaichi
 
Ok, I got it figured out thanks to Caddie's help. I did steps 1-3 above in Caddie's response. I couldn't get step 4 to work so I did a rip connect from the SMT Conversion. That worked and I was able to flatten the piece
smiley32.gif
. I will post the complete part this evening in case someone can learn from my experience.


Now, I need to make this part. I flattened the image but it doesn't give me dimensions, only some angles and the thickness. From my solid modeling experience, I could go into sketcher mode and could find out whatever dimensions I needed. Is there a way to get the dimensions of the part flattened out?


Thanks again for everyones help on this, it's greatly appreciated,


Craig
 
If you mean "retrieve" dimensions then this is not possible. You can measure the flattened state any way you want and you can create a drawing for it. Just make the flattened state an instance of the part and select the flattened state as model for a drawing view. Then you take all relevant dimensions from the drawing view.


Retrieving dimensions is only possible for those dimensions that are parameters for the model. Since you start with the finished part, you can only retrieve those dimensions. If you would start with the flat sheet and create a sheet metal part by inserting bends then you would have the sheets dimensions available, but consequently you would then need to dimension the finished part by hand. In my experience entire parts are (almost) never modelled out of the flat sheet. Bending out detailed cuts however is a common practice.


Alex
 
I have a similar issue with a solid part that was designed in Wildfire 1.0. I am also new to using the sheetmetal module.



When I tried creating a sheetmetal conversion, I received error
messages regarding the edge rip. Can someone show me the correct way to
do this?



Thanks for your help.


2005-11-08_001626_sm_concept-1.zip
 
I find the best way to manage flat state dimensions is to create ref
dimensions by surface in part mode after the part has been flattened
and then show these (dimensions) on the drawing.





DB
 
Dell_boy,


are there any advantages in creating the dimensions in part ? I would create dimensions in draft, they are references anyhow so you have to create them where you need them.


Alex
 
The main advantage of creating dimensions in part mode is that you only
have to do them once. If you change your mind about a view (delete, turn over,
re-orient or different instance) you only have to re-show the dimension
as opposed to having to re-create it. This is even more of a hassle when you want to embed a note in the dimension or such as



"{0:developed length = }{1:mad:D[.1]}{2:mm based upon }{3:&inside_rad}{4:mm inside radius}"



You can also used the fully developed length to drive other parameters or appear in a note or B.o.M.



and I hate creating dimensions in draft.





DB



Edited by: Dell_Boy
 
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