Can I offset lines in a sketch

[cad fool]

Can I offset lines in a sketch without having a model in it. In solidworks you can offset lines when sketching in a new sketch (before an extrude) Can you do the same using Pro-E?

 

[appinmi]

Yes, on the sketch toolbar, there is a button for "use edge". Select the arrow next to it and select the button "Offset edge". You now hav the option to select one edge at a time, or a chain of edges.

 

[cad fool]

Thanks for your help, I know this can be done. The command says "select an edge", an edge of what? an edge of a pre-exsisting model. What I am talking about is offsetting lines without the use of a pre-exsisting model

 

[appinmi]

That is he only way that I know of. You could create a datum curve for the first entity. Then create your feature with "use edge", select the entire curve chain, and "offset edge", select the entire curve chain again.

 

[csusie]

You can offset pre-existing geometry. This geometry could be solid, surface or curves.


"What I am talking about is offsetting lines without the use of a pre-exsisting model"


You need to have something in order to do an offset otherwise what is an offset.

 

[dross]

You can offset pre-existing geometry. This geometry could be solid, surface or curves.


"What I am talking about is offsetting lines without the use of a pre-exsisting model"


You need to have something in order to do an offset otherwise what is an offset.

He is referring to the offsetting of lines within sketcher only, similar to drafting in a 2-D CAD program such as autocad.


As far as I know, it's not available in ProE. Just draw your lines and change the weak dimensions to what value you need. That was the hardest thng for me to grasp when I made the switch from AutoCAD to ProE, it just seems foreign.


You'll get used to it.

 

[michaelpaul]

Can I offset lines in a sketch without having a model in it. In solidworks you can offset lines when sketching in a new sketch (before an extrude) Can you do the same using Pro-E?

nope, that's just one of the many things that you cannot do in Pro that you could do in SW.

I find myself sketching my profile and then using a lot of construction lines of equal length to create my new "offset" sketch around the original. It's a work around but it gets the job done.

Basically I'll create my first profile and then my second profile. I'll connect the two proviles with a construction line perpendicular to each profile. I'll set all the construction lines equal to one another so that at each point it's the same distance away from the first profile. it takes some time to get right but once it's set up then you have effectively created an offset sketch.

Michael

 

[elab.theken]

Why not just create the first profile as a datum curve and then offset a second sketch? You might have two features in the model tree, but if grouped I don't see much of a down-side.

 

[michaelpaul]

Why not just create the first profile as a datum curve and then offset a second sketch? You might have two features in the model tree, but if grouped I don't see much of a down-side.

that would certainly work. it's just one of the things I hadn't thougth about so I I did it my way. I'll probably start doing it this way though since it is a bit more flexible.

personally I don't like groups though because I don't like it when a model has a lot of groups and I'm trying to click a feature in the model and see where it is in the model tree. if it's embedded in a group the group won't highlight so you have to expand your gruops to see the feature highlighted. kind of a pain.

thanks for the tip though.

Michael

 

[burnsp]

On that note about highlighting, is there any way to make the group highlight (instead of just the feature) when you select a featurefrom the model?

 

[SW]

To get the group to highlight in the model tree, right-click and use the "Select Group" option.

Sam

 

[vlad1979]

There is a way to offset the sketch. Not a real offset but it works.


Select all that you want to offset, then edit/copy and drag the sketch to adjust the scale and then place it.


2006-10-02_014417_COPY_SKETCH.rar

 

[giridhar_tech]

and moreover,


I could also not find the array command in Skectcher,


Can anybody commnet.

 

[SW]

Its generally accepted to try and keep sketches simple, so the lack of an "array" command within the sketcher is understandable. Create your sketch, then use the pattern command.

Sam

 

[pjw]

You can do what you're asking for easily. Creat a sketched datum curve prior to any offsets. You will only need to sketch it one. Then, select your datum curve and use the 'Edit' 'Offset' command. Select the plane in which to offset. You will only have one offset dimension. See attached picture.





Does this help?View attachment 2753

 

[rchinnap]

The downside of using offset feature would be, you cannot use them on sketch based feature. If you want then you have to use-edge them.. creates more Parent/Child relation ship.

 

[pjw]

Of course you can use them on sketch based features. That's what the example I've shown you is. To offset edges from solid geometry you would first need to copy the edges with a composite datum curve. Don't worry about features in the model tree. Too many people place too much importance about how many features there are. Remember - it's important that you end up with the geometry you set out to accomplish and provided the model is robust and has been produced with a bit of thought then it really doesn't matter how many features there are which make it up. Using the offset in the above example is actually better than using only one sketch and offsetting 'use edge'. Many people will know that 'use edge' creates a lot of references in the sketcher. When the number of references becomes great the performance of sketcher is greatly affected - as in the case of 'use edge' for creating protrusions from sketched text datum curves.


Phil

 

[pronto_1]

you can use the copy paste cammand. select whatever you want to offset -> edit-> copy->edit-> paste. then drag the line to whereever you want.