How do you extrude only a part of a sketch.

[DesignIntent]

I have been trying to extrude only one or two lines of a complex sketch and can't seem to prevent the entire sketch (or contours) from being selected.
I have created a large sketch which I use as a master for multiple solids within one part file, similar to what the Pro-E people do.
I do not want to add these individual lines to secondary sketch using "convert entities".
This defeats the purpose of having all the control in one sketch.
Any thoughts?
Thanks

 

[TheTick]

This defeats the purpose of having all the control in one sketch.

No it doesn't. It just adds another step. Not even a big one. Call it a "SolidWorkaround".

 

[DesignIntent]

I must beg to differ that generating multiple secondary sketches into which portions of geometry are added via convert entities is not a hit to efficiency and time.
In this case, more than 45 secondary sketches would have to be created to support the content of the part design i am creating.
There is also a similar need for extruding and/or revolving new solids and/or surfaces using edges of existing solids.
I do high flow intake design which requires the joint input from both a master sketch and resultant edges of the generated solid model that cannot be modeled directly.

This can be done in both Unigraphics NX and Catia and even Proe-E but it seems Solidworks does not have this capability.

Still looking for some help with this issue.

 

[drawoh]

DesignIntent,

One of the things I do in SolidWorks is create a layout sketch, possibly in 3D. I never extrude or rotate the layout sketch. I use it to control the geometry of all the other sketches. This can be done at the assembly level. If the layout sketch is embedded in a layout sketch file, it is accessible from outside your assembly.

--
JHG

 

[hendersdc]

They are different tools with different capabilities, to the best of my knowledge solidworks cannot do what you are asking. The easiest way to create the design off of a reference sketch in solidworks is to use convert entities.

 

[TheTick]

Making sketches is not hard. If it is, you need training and practice.

Derivative sketches add nigh-zero overhead in regeneration time.

If a "layout" sketch is so well-refined that there is zero editing to do of downstream feature curves, it probably has too much detail.

How does one trim or extend a curve from a layout sketch without adding it to another sketch?

I've worked in Pro/E. I'm working in NX today. If you've worked in NX or Pro/E, then you should be quite accustomed to workarounds.

SW has some shortcomings. Nearly all are manageable with patience and skill (the same patience and skill one needs in other CAD).

 

[DesignIntent]

I thought I would try to show an example pictorially of what I mean in the event someone has a trick Ive not found yet.
Some times a picture better communicates the concept.

I am trying to accomplish this is for one of my customers who uses Solidworks and need to pass the file on to them so they can continue.


By the way, I have 30+ years on NX and 10+ years on Pro-E and I have owned Solidworks since version 2000.
And I have found the solutions to many problems like this by asking questions.
I'm not a novice, just need a little help from the community.
We all don't know everything.

 

[RobLN]

Hi
Modelling from a highly thought through initial sketch is great and it does save time further down the line. Within NX you can also wave link the sketches adding more functionality to the whole design.

Whilst I understand that you can use this technique it does require a degree of understanding from the whole team. And from experience having had to work on such models made with multiple extruded features from a single sketch it is very easy to get confused and for the entire model to fail almost impossible to repair. In my view you should stay with the functionality of SolidWorks (ie single sketch - multiple solids is not advisable) and use the KISS approach..

One advantage of Solid Works over NX is that the projected curves (convert entities) seems to be associative by default whereas in NX this tends to be more hit and miss...

BR

Rob

Solid Edge; I-Deas 7 to 12; NX4 to NX8.5 / TeamCenter 9.1 & Ansys 14.5 / SW 2016 - 2018

 

[FACS]

Is it possible that you can use sketch Equations to accomplish this?

 

[TheTick]

@OP You've obviously been around and have done quite a bit. I know you just wanted an answer. Sorry for trolling.

The short answer is "No, SW won't do that." That is, for basic features like revolves and extrudes. For lofts and sweeps... well... some exceptions can be made.

I'm more compelled to challenge the assertion that this shortcoming "...defeats the purpose of having all the control in one sketch". Hardly. Control is control, even if it's removed by an degree or two.

Workaround or not, adding new sketches for features adds a degree of robistitude to models that can save a model or project. When modeled this way, it's possible to outright replace an entire series of layout sketches without exploderating the whole spiel.

 

[drawoh]

DesignIntent,

Definitely, draw your sketch at the assembly level. Use it to control the extrusion and rotation sketches on the parts.

I have no experience with the other 3D CAD packages other than Mechanical Desktop. In SolidWorks, if the part is not absolutely simple, I define it as an assembly. The assembly is what I attach to the fabrication drawing. This allows me to tell the fabricator to attach dowel pins and thread inserts. I can also create a part, excluded from the BOMs that does nothing other than hold your layout sketch. This is attached to each of your part assemblies, and your parts can be worked on by two different designers.

--
JHG

 

[DesignIntent]

Thank you all,

I changed my approach and got what I need.
Too bad about the base capability in SW.
Did not mean to criticize the software.
But I did learn from all of this an additional method that will work.
Would not have noticed it were it not for the input from everyone.

FYI....
I am now using a master sketch built in a top assembly and push the control to component files.
Makes a small extra step but it will do.

Thanks again.

D.I.

 

[SwinnyGG]

DesignIntent,

Definitely, draw your sketch at the assembly level. Use it to control the extrusion and rotation sketches on the parts.

I have no experience with the other 3D CAD packages other than Mechanical Desktop. In SolidWorks, if the part is not absolutely simple, I define it as an assembly. The assembly is what I attach to the fabrication drawing. This allows me to tell the fabricator to attach dowel pins and thread inserts. I can also create a part, excluded from the BOMs that does nothing other than hold your layout sketch. This is attached to each of your part assemblies, and your parts can be worked on by two different designers.

This sounds like a PDM nightmare.. how do you handle naming/revision control of a bunch of sub parts that aren't actually parts, but are really just features of a part?

 

[TheTick]

IF your “parts” are just features of other parts, why not make a multi-body part?

 

[drawoh]

jgKRI,

Fabrication drawing 123-456 is linked to a tree of CAD models. If any of those models are changed, drawing 123-456 must be updated. We are back to the old rule about not changing form, fit or function. Any chaos you inflict on the CAD[ ]model probably is chaos out on the production floor.

At the assembly drawing level, you have to be tolerant of outdated models attached to the tree, but the form, fit and function rule still applies.

--
JHG

 

[drawoh]

TheTick,

I want to attach helical thread inserts, PEM nuts and Riv-nuts from a library. I want a consistent description on the BOMs on the fabrication drawings. I want a BOM on the fabrication drawing so that the fabricator does not charge me for the time he wastes finding out he needs hardware.

Can I do a multi-body sheet metal part, and make flat layouts of the pieces?

SolidWorks' weldment feature can be used creatively, but it has its limits.

--
JHG

 

[SwinnyGG]

Fabrication drawing 123-456 is linked to a tree of CAD models. If any of those models are changed, drawing 123-456 must be updated. We are back to the old rule about not changing form, fit or function. Any chaos you inflict on the CAD model probably is chaos out on the production floor.

After further thought, my expectations of this method being troublesome are dissipating quickly. It's an interesting approach actually.

Are you using a true PDM system or managing all of this stuff manually?

 

[drawoh]

jgKRI,

I am used to PDM. When you check in your drawing, PDM normally checks in everything attached to it.

--
JHG

 

[SwinnyGG]

Yeah if it's automated there's less to track. Could be useful for managing certain types of configurations.

I'm thinking I might try this actually.. I have some new people coming on in the next month, and was already concerned about allowing one of them who have little or no experience access to full models with important configurations in our system that should not be altered.

With this method I could allow them to work on parts but only access specific features (or sets of features). Which could be highly valuable.

 

[drawoh]

jgKRI,

That sounds way more complicated, and I don't think PDM will do it. What it will do is recover the old model after your new person messes it up.

--
JHG