In SE, is there a quick way to

[prsyam]

Since I have switched from Solidworks to SE-ST5,I am facing following issues, still I can ignor all this (even if there is no solutions) since SE really made my time worth.
#1. Create a plane middle to two surface (select two surface & got a plane in the middle) Eg. DIN-332 center holes on both side of the shafts, etc…
#2. Give tolerence to the hole and slot dimentions in Part enviroment, because I would like to retrive all dimentions with tolerence from master instead of giving it in drawing.
#3. Giving two material in one part (Eg. PU coated Roller). I know it is diffcult but atleast like "Not Merge" option in Solidworks. so that I can demonstrate in drawing manually.
#4. CSK holes with a depth before the hole, It is very common to give 1mm depth & SW is giving this option.
#5. Copying all associated files along with the assembly in one folder. Like SW Pack & go.
#6. Make a cover transperent to see what is inside sometime it is necessory to see something is interfering with the cover itself.
Thanks

 

[KENAT]

#2. Give tolerence to the hole and slot dimentions in Part enviroment, because I would like to retrive all dimentions with tolerence from master instead of giving it in drawing.

Because SE is only one way associative this doesn't work as well as in programs like SW. It's been a while since I tried doing this and I can't remember exactly how it went - certainly didn't work well enough to do it all the time for me.

#5. Copying all associated files along with the assembly in one folder. Like SW Pack & go.

There is a utility called Revision Manager that comes with Solid Edge (unless something has changed) this is the best way to do file manipulation.

#6. Make a cover transperent to see what is inside sometime it is necessory to see something is interfering with the cover itself.

Changing face style to white glass or similar should help. You can also run interference checks & inquire minimum distances.

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[kjoiner]

#1 - ST5 has a center plane for assembly relationships, but I'm not sure if it has one for part.

#2 - You can use the PMI dimensions to call out tolerances in the part. Once you place the dimension, you can click on it and then use the "modify dimension type" to enable to type of tolerance you want (± or limits etc.). You can then retrieve dimensions in the detail drawing.

#3 - If you have an overmolded part, it's really best to create it as an assembly since that is how it is done in manufacturing.

#4 - Can you provide a little more information on this one?

#5 - As Kenat mentioned, Revision Manager is the best tool for that. You will also need to use Revision Manager when moving files, renaming etc. to maintain the links properly.

#6. As Kenat mentioned - change the face style to a transparent one. There are several including blue, green, red and white glass.

Kyle

 

[prsyam]

Dear All, Thanks for your time, I think I am enlightened in #2 & #5
#1 DIN332 Center hole includes one hole and a revolved cutout
If I can make a plane at the middle of the shaft driven by it's two end, along with this two feature so many other features can be mirrored thus avoid the redundant dimensions in drawing when retrive from part file.
#3 kjoiner is correct if we have the expertise and time in making the overmoulded parts, but our practice is to give only one drawing to Vendor and it was their cup of tea to design and make it.
I was able make drawings in SW with "No Merge" option in extrude and hatch manually according to the material. I mentioned that giving material to get exact weight is not a big concern.
#4 One flat bottom simple hole with ~1mm depth and CSK dia., then CSK hole from the bottom of that hole.
This was one feature in SW.
#6 I managed to do this way
(Select cover > View > Styles > Select any glass style > Apply) or
(Select cover > View > Face Overrides > Appearence > Reduce Opacity > Apply),
but for both I am unable to remove the override, all this was single click in SW.

 

[KENAT]

I haven't looked at the ST interface for a while but in older versions when you select a part in an assy you should see a window up on the toolbar that says what the 'color' of that part is. Then with a pull down you can easily change to a default glass one. If they've made it harder in ST that's a bit silly.

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[prsyam]

Hi All, I am thankful to my friend for solving the issues of #3, #4 & #6 as follows
#3 "Add body" feature under solids will do this.
#4 This kind of CSK holes can be made with counter bore hole option with V-bottom angle checked.
#6 I dont know how I left a dropdown menu on the left side of face override botton unnoticed.
So the only remaining point is #1

 

[Spaceballster]

You cannot create a plane between two surfaces without a helper. Quickest way is to probably make a new sketch, draw a line between the two surfaces. Exit the sketch, and create a plane "Normal to Curve". You can then type in 0.5 and you will have a plane in the middle of the line. (this is on ST4 btw)

 

[Spaceballster]

Oh yeah, any questions asked about SE involving the word "quick" is probably most of the time not possible.