Northlandhusky
Mechanical
Does anyone knof if in V5, there a quick way to do a V4 transform move (axis to axis,) within the connstraints or other area, or is it neccesary have to do several zero length offsets to position parts.
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V5 - Trasform move equivalent ??
- Thread starter Northlandhusky
- Start date
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belvedere64
Automotive
In an open body named inputs or drivers, have points locating parts.
In the same open body create mount hole centerlines from these points.
In the part body constrain to these resulting centerlines
When your nieghbor wants to know where your mount locations are, publish only the lines
When you need to move your part edit the point properties
Use your power only for good, never evil
In the same open body create mount hole centerlines from these points.
In the part body constrain to these resulting centerlines
When your nieghbor wants to know where your mount locations are, publish only the lines
When you need to move your part edit the point properties
Use your power only for good, never evil
- Thread starter
- #3
Northlandhusky
Mechanical
I FOUND THAT IT CAN BE DONE USING SCENES VERY EASILY AND THEN APPLYING THE SCENE TO AN ASSEMBLY. A LITTLE CONVOLUTED BUT IT GETS THERE.
In the assembly design toolbench, there is a command called "snap to". The icon reminds me of a pawn in chess. If create axes in the individual CatParts you can use the snap to command to move one part to another similar to V4-Transfor-Move.
- Thread starter
- #5
scottriley
Aerospace
In GSD there a is a transformation function called 'axis to axis'. This works almost exactly the same as in V4
cullensimpson
Computer
I have found that the GSD axis to axis creates a volume and leaves the transformation in the tree rather than simply moving the solid/surface/whatever from V4.
Any way around that?
Any way around that?
the only way so far is to use the compass, but this will work only with isolated elements (point,curve,line,surface,plane,solide) with no history. Everything link to those elements will move according to their definition be carefull.
It is not as easy as in V4 to move a real V5 solid because of all the links you can have... Parametric is here !!!
I notice that using the compass to move geometry within a part might not work if you work under a product... at least the first move.. this is a bug.
So the steps are :
a part alone with isolated elements:
1) create 2 axis (starting and ending position)
2) put the compass wherever you wantcompass turns green
3) make the starting axis the active one
4) press escape ( = unselect) compass turns white
5) double clic the compass or edit
6) key 0,0,0 for the position of the compass and move
7) nothing else than the compass should move
8) the compass is at 0,0,0 of the starting axis
9) select ending position axis and make it active compass turns green
10) new coordinat are shown in the compass edit box
12) unselect (escape) compass turns white
13) select element you want to move compass turns green
14) key 0,0,0 and move
What a workaround !!!
a part under a product with isolated elements:
1) create 2 axis (starting and ending position)
2) put the compass wherever you wantcompass turns green
3) make the starting axis the active one
4) press escape ( = unselect) compass turns white
5) double clic the compass or edit
6) key 0,0,0 for the position of the compass and move
7) nothing else than the compass should move
8) the compass is at 0,0,0 of the starting axis
9) select ending position axis and make it active compass turns green
10) new coordinat are shown in the compass edit box
11) unselect (escape) compass turns white
12) select elements you want to move compass turns green
13) make a move 1 mm (or in) along one direction (x,y or z)
14) the compass only moves not the geometry = bug
15) key 0,0,0 and move geometry the compass move to ending axis but geometry is 1mm (in) away
16) move back 1 mm or in along the same direction
17) geometry is in place but not the compass
Thank you CATIA V5 !!!
Eric N.
catiav5@softhome.net
It is not as easy as in V4 to move a real V5 solid because of all the links you can have... Parametric is here !!!
I notice that using the compass to move geometry within a part might not work if you work under a product... at least the first move.. this is a bug.
So the steps are :
a part alone with isolated elements:
1) create 2 axis (starting and ending position)
2) put the compass wherever you wantcompass turns green
3) make the starting axis the active one
4) press escape ( = unselect) compass turns white
5) double clic the compass or edit
6) key 0,0,0 for the position of the compass and move
7) nothing else than the compass should move
8) the compass is at 0,0,0 of the starting axis
9) select ending position axis and make it active compass turns green
10) new coordinat are shown in the compass edit box
12) unselect (escape) compass turns white
13) select element you want to move compass turns green
14) key 0,0,0 and move
What a workaround !!!
a part under a product with isolated elements:
1) create 2 axis (starting and ending position)
2) put the compass wherever you wantcompass turns green
3) make the starting axis the active one
4) press escape ( = unselect) compass turns white
5) double clic the compass or edit
6) key 0,0,0 for the position of the compass and move
7) nothing else than the compass should move
8) the compass is at 0,0,0 of the starting axis
9) select ending position axis and make it active compass turns green
10) new coordinat are shown in the compass edit box
11) unselect (escape) compass turns white
12) select elements you want to move compass turns green
13) make a move 1 mm (or in) along one direction (x,y or z)
14) the compass only moves not the geometry = bug
15) key 0,0,0 and move geometry the compass move to ending axis but geometry is 1mm (in) away
16) move back 1 mm or in along the same direction
17) geometry is in place but not the compass
Thank you CATIA V5 !!!
Eric N.
catiav5@softhome.net
cullensimpson
Computer
I am really looking for a way to do this in VB, but you do not have access to the compass there.
I can not find an equivalent to the snap command in VB either.
The axis to axis is unacceptable since it creates a volume.
I could use translate and a series of rotates. I have the transformation matrix that needs to be applied, but the rotate calls are looking for angles rather than a matrix.
I have not found a method to convert from the matrix to angles about each axis that I can grasp.
Thoughts?
I can not find an equivalent to the snap command in VB either.
The axis to axis is unacceptable since it creates a volume.
I could use translate and a series of rotates. I have the transformation matrix that needs to be applied, but the rotate calls are looking for angles rather than a matrix.
I have not found a method to convert from the matrix to angles about each axis that I can grasp.
Thoughts?
Hi!
Another tip on how to move geometry:
-hide the default planes in CATPart(XY,YZ,ZX)
-create a point in 0,0,0
-put an axis system on this point
-use the planes on the axis system to create your geometry
-when you will move the geometry, just change the values of the point and play with your axis system
Regards
/Yngve
Another tip on how to move geometry:
-hide the default planes in CATPart(XY,YZ,ZX)
-create a point in 0,0,0
-put an axis system on this point
-use the planes on the axis system to create your geometry
-when you will move the geometry, just change the values of the point and play with your axis system
Regards
/Yngve
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