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CATIA V5 best practices 5
- Thread starter jay24
- Start date
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here's a few tips that are open to discussion:
1. always fully constrain sketches (sketches should be green or yellow - never white)
2. always do a sketch analysis before you exit a sketch
3. limit the use of boolean operations
4. when working with assemblies (products), always use SAVE MANAGEMENT (if not using a PDM)
5. always publish elements that will be linked to child parts, and only make external references to published elements
1. always fully constrain sketches (sketches should be green or yellow - never white)
2. always do a sketch analysis before you exit a sketch
3. limit the use of boolean operations
4. when working with assemblies (products), always use SAVE MANAGEMENT (if not using a PDM)
5. always publish elements that will be linked to child parts, and only make external references to published elements
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Hi,
When you create a Hole on a non-planar face of a solid :
Create a point on the surface, the axis of the Hole and a plane normal to the axis passing thru the point.
Then Pre-select the point and the plane when you create the Hole.
In other words: when you create a Hole on a surface, never clic on the surface!!!
Eric N.
catiav5@softhome.net
When you create a Hole on a non-planar face of a solid :
Create a point on the surface, the axis of the Hole and a plane normal to the axis passing thru the point.
Then Pre-select the point and the plane when you create the Hole.
In other words: when you create a Hole on a surface, never clic on the surface!!!
Eric N.
catiav5@softhome.net
Hi,
To create a new exemplar of a CATPart based on an existing one it is very important to use “File/ New From” command and not “Save As” command! “New From” creates a new exemplar of an existing one and prevents problems in the product structure.
Never use planar surfaces (its better to use planes) for sketch support because its easier for changing the sketch- support if you want to make some modifications.
For better performances in creation of a catpart, features like fillet, chamfer, draft, shell a.s.o. should be used whenyou finish the catpart, so these features will be at the endof the specification tree.
Keep sketch as simple as possible to make modifications easily. Don’t create geometry which can be created as features, i.e. fillets, chamfers, holes. Don’t use mirror function in Sketcher, use it in Part Design.
Auxiliary elements have to be created as construction elements because otherwise the
sketch doesn’t work correctly
Use Auto Search command to select all elements of a sketch profile easily. Select only one element of the profile and run Auto Search with the right mouse button .
Use Auto Constraint command to constraint the whole sketch easily.
Regards
Fernando
To create a new exemplar of a CATPart based on an existing one it is very important to use “File/ New From” command and not “Save As” command! “New From” creates a new exemplar of an existing one and prevents problems in the product structure.
Never use planar surfaces (its better to use planes) for sketch support because its easier for changing the sketch- support if you want to make some modifications.
For better performances in creation of a catpart, features like fillet, chamfer, draft, shell a.s.o. should be used whenyou finish the catpart, so these features will be at the endof the specification tree.
Keep sketch as simple as possible to make modifications easily. Don’t create geometry which can be created as features, i.e. fillets, chamfers, holes. Don’t use mirror function in Sketcher, use it in Part Design.
Auxiliary elements have to be created as construction elements because otherwise the
sketch doesn’t work correctly
Use Auto Search command to select all elements of a sketch profile easily. Select only one element of the profile and run Auto Search with the right mouse button .
Use Auto Constraint command to constraint the whole sketch easily.
Regards
Fernando
jay24:
-Keep your tree well organized and take the time to rename the elements to something that makes sense. It will make it easy on anyone else that uses your file.
-Give a lot of thought to applying relationships and constraints. They can cause you, or whoever has to update/modify your file, a lot of grief if not carefully created.
Terry
-Keep your tree well organized and take the time to rename the elements to something that makes sense. It will make it easy on anyone else that uses your file.
-Give a lot of thought to applying relationships and constraints. They can cause you, or whoever has to update/modify your file, a lot of grief if not carefully created.
Terry
Ferdo...
What's wrong with using Mirror inside a sketch?
I do it all the time. A simple example is two parallel lines that are centered about an axis. Sketch one line and the axis, then mirror the second line. Constrain the total distance between the two lines. Works great!
...Jack
What's wrong with using Mirror inside a sketch?
I do it all the time. A simple example is two parallel lines that are centered about an axis. Sketch one line and the axis, then mirror the second line. Constrain the total distance between the two lines. Works great!
...Jack
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I think there is nothing wrong with using the mirror inside the sketch also I don't think there is anything wrong with using radii in a sketch(instead of fillets) it's very easy to change the radii in a sketch and a lot of times using fillets outside the sketch makes the geometry very heavy and complex.
It all depends on the case if I have a simple extrusion like a gasket why would I use fillets???
However in more complex designs it might be more useful designing to hard corners and fillet afterwards.
Think before you design, rules don't work all the time (but it can give you a good direction).
I also heard a lot of times that converting from Catia v4 to Catia v5 is soooo difficult, thats bullshit if you were a good designer in v4 able to use solids it should not be that difficult.
The hardest thing to overcome as a v4 user was the links and doing packaging because we were not used to the assembly structures like they have had in Unigraphics for a long time.
It all depends on the case if I have a simple extrusion like a gasket why would I use fillets???
However in more complex designs it might be more useful designing to hard corners and fillet afterwards.
Think before you design, rules don't work all the time (but it can give you a good direction).
I also heard a lot of times that converting from Catia v4 to Catia v5 is soooo difficult, thats bullshit if you were a good designer in v4 able to use solids it should not be that difficult.
The hardest thing to overcome as a v4 user was the links and doing packaging because we were not used to the assembly structures like they have had in Unigraphics for a long time.
I agree with JuhaEdag.
I can see no logic to putting fillets/chamfers outside the sketch. Sounds like carry over methodology from V4 to me.
We design a lot of machinings with complex revolutions and it is far easier to see all the chamfers/fillets in one sketch.
I can see no logic to putting fillets/chamfers outside the sketch. Sounds like carry over methodology from V4 to me.
We design a lot of machinings with complex revolutions and it is far easier to see all the chamfers/fillets in one sketch.
Actually, the beauty of sketches is that you can change it so if your'e not happy with it take the bloody corners off!
Like I said think before you design it all depends on application. The Gasket was maybe a bad example ( because I never done one my self) but I would imagine it is cut by some kind of stamping tool (what is the draft used for then?).
I have worked in BIW, Interior design, I-P design, A-class surfacing, Seatings and recently Electrical design and I still think if you can incorporate your fillets in the sketch you will have one less of operation to worry about.
However like I said before it all depends on application if you have deep draws you would of course design to hard corners then draft your surfaces (solid walls) and fillet.
There is many applications though where you can sketch with corners (i.e you have two sketches and you run a surface or a solid to create your shape between the sketches, First sketch is much larger than the second this will give you draft naturally, why in the world would you want to add draft when you already have draft by the shape? it would be easier to change the shape of one of the sketches to allow more draft).
It all depends on application don't misunderstand me I use shapes without fillets all the time especially in moulded plastic parts but if I can incorporate it into my sketch I'm happy it makes updating easier and in the end I will have enough fillets to fight with for sure (no xtra needed).
Like I said think before you design it all depends on application. The Gasket was maybe a bad example ( because I never done one my self) but I would imagine it is cut by some kind of stamping tool (what is the draft used for then?).
I have worked in BIW, Interior design, I-P design, A-class surfacing, Seatings and recently Electrical design and I still think if you can incorporate your fillets in the sketch you will have one less of operation to worry about.
However like I said before it all depends on application if you have deep draws you would of course design to hard corners then draft your surfaces (solid walls) and fillet.
There is many applications though where you can sketch with corners (i.e you have two sketches and you run a surface or a solid to create your shape between the sketches, First sketch is much larger than the second this will give you draft naturally, why in the world would you want to add draft when you already have draft by the shape? it would be easier to change the shape of one of the sketches to allow more draft).
It all depends on application don't misunderstand me I use shapes without fillets all the time especially in moulded plastic parts but if I can incorporate it into my sketch I'm happy it makes updating easier and in the end I will have enough fillets to fight with for sure (no xtra needed).
I'm truly Sorry I thought we're talking about making the parts from 3-d data. Sorry about my ignorance but last time I did a drawing was in Italy 2000 and It was so boring doing all those mega drawings (to make managment happy), fortunately v5 seems to be aiming to get rid of most of it!
Whatever works best for the situation. If I am doing a 2D shape that is being extruded or cut out with a laser or even simple shears then go ahead and put in the fillets(gaskets and such). If I am doing something a little more complex then hold off on putting them in the sketch. Alot of times the fillets need to be deactivated to ship to an analysis group. The order that they are applied can be critical as well. Never fillet then draft. If you do the fillet is no longer a true radius. Things like that.
arvindsathe
Automotive
What is Catia Publish?
Why is it important to make external references (for child parts) only to published data?
Why is it important to make external references (for child parts) only to published data?
MGONZALEZ41
Mechanical
DOES ANYONE KNOWS HOW TO EDIT THE TITLE BLOCK AND BILL OF MATERIALS WITHOUT USING A MACRO, ANS STILL KEEP THE LINKS TO THE COMPONETS AS PART NO., DESCRIPTIONS AND SO ON.
THANKS.
THANKS.
Arvindsathe....
Publish provides several advantages over non-published links, but the biggest is when you do changes to the parent part. If the parent part is replaced or renamed or if the published geometry is replaced, the links will be maintained and the child parts will remain in-sync. Non-published references must be replaced manually.
Publish provides several advantages over non-published links, but the biggest is when you do changes to the parent part. If the parent part is replaced or renamed or if the published geometry is replaced, the links will be maintained and the child parts will remain in-sync. Non-published references must be replaced manually.
Hey MGONZALEZ41
You have to Attributes links:
1-During the text edition, right-click on the background and select Attribute link
2-Activate the 3D document and select the component witch you want to read the value from.
3-Back in the 2D, select the appropriate attribute/property from the available list.
Good luck
SaP
You have to Attributes links:
1-During the text edition, right-click on the background and select Attribute link
2-Activate the 3D document and select the component witch you want to read the value from.
3-Back in the 2D, select the appropriate attribute/property from the available list.
Good luck
SaP
Configurator
New member
Keep sketches simple. V5 is FEATURE BASED. I can handle complex sketches, but it will bog down the system. I often have nothing more than a line in a sketch.
This should be obvious, but I see it a lot, so here goes: Don't use windows to re-name, copy or move files. You're begging to screw up UUIDs (and thus links) if you do so.
Work with cache if you have large assemblies.
Someone mentioned booleans above. Avoid them when they aren't necessary (ie: do a pocket instead of a remove, etc.).
I disagree with ferdo on this one: don't use auto-constraints. It's best to explicitly define everything yourself.
The main thing is to be aware that in parametric modeling systems, everything is kept track of.
This should be obvious, but I see it a lot, so here goes: Don't use windows to re-name, copy or move files. You're begging to screw up UUIDs (and thus links) if you do so.
Work with cache if you have large assemblies.
Someone mentioned booleans above. Avoid them when they aren't necessary (ie: do a pocket instead of a remove, etc.).
I disagree with ferdo on this one: don't use auto-constraints. It's best to explicitly define everything yourself.
The main thing is to be aware that in parametric modeling systems, everything is kept track of.
Avoid links between parts in an assembly. Use skeleton parts if you want to use linked parameters and geometry. Links like this makes Catia slow. Important when you work with large assemblies.
Constrain your sketch to the planes and not to H and V axis (the big yellow ones).
Always use a positioning part (a part containing plans etc as reference when positioning other parts) in your assemblies. Add a "Fix" constrain to it. This makes eveything fixed to the "absolute" coordinate system of the assembly.
As said before, only link published geometry/parameters.
If you make the links from a skeleton and a part when they are in the same context the pointing feature of the link is shown in the name of the link.
Only sketch on planes (not planes that are created with any reference to the solid or surface) not on a face or a surface. This will make your model more stable if you would like to make changes to it.
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