AnsweredAssumed Answered

How to hide base sketch in skeleton sketch method?

Question asked by Tom Hickerson on Jul 10, 2017
Latest reply on Jul 11, 2017 by Matt Peneguy

Like • Show 1 Like1
Comment • 16

I am trying to use skeleton modeling. I have a skeleton part that is just a 3d sketch. I want to use that for my other parts and assemblies to control their dimensions and mates.

I opened a new part and did insert part, and picked the skeleton part, and choose unabsorbed sketches. I wanted to use it as a basis for a weldment. I added a sketch on top of the skeleton part, and that all works fine. Now I want to hide the skeleton part sketch. However the eyeball doesn't appear in the choices for this part like it usually does.

I can however edit the 3d sketch (the new one not the skeleton part) and right click on one of the lines and choose hide and it goes away. However I can't figure out how to make it visible again if I need to.

Am I going about this all wrong?

No one else has this question

Outcomes

16 Replies

S. Casale Jul 10, 2017 4:14 PM
Mark Correct
Correct Answer
John Stoltzfus May be one of the best to answer...
Like • Show 3 Likes3
Actions
Dennis Dohogne Jul 10, 2017 4:36 PM
Mark Correct
Correct Answer
Make sure you are out of the sketch. RMB on the sketch in the Feature Manager Tree and select Hide.
Like • Show 4 Likes4
Actions
Dan Pihlaja Jul 10, 2017 4:49 PM
Mark Correct
Correct Answer
1) Normally I don't use Insert part when using skeleton sketch. I insert the skeleton part into a main assembly and then the part that I want to create from it into the assembly as well. Then use in context modeling to link the part to the skeleton part.

2) If you still want to do it your way (which is a fine way of doing it by the way), you can hide those sketches, but only by selecting them in the feature tree and using the hide column (click the little double arrows at the top right of the feature tree).
Like • Show 3 Likes3
Actions
- Tom Hickerson @ Dan Pihlaja on Jul 10, 2017 5:24 PM
  Mark Correct
  Correct Answer
  Dan,
  I just googled the in context modeling. Its my understanding that you insert new part, or new assembly into the model with your skeleton part? Is that correct?
  Like • Show 2 Likes2
  Actions
  - Jim Steinmeyer @ Tom Hickerson on Jul 10, 2017 6:05 PM
    Mark Correct
    Correct Answer
    Tom,
    The way I do it is to create a skeleton sketch part. Then create a new assembly and place the skeleton part in it. Now I will go to Insert>Component> New Part/ or New Assembly. This will allow you to create the new part or assembly inside the assembly using the skeleton part sketch for your dimensions and locations. When finished the part can be saved as virtual which exists only with in assembly, or you can save it out as an external part so it will show in your folders and be able to be used somewhere else.
    
    A word of caution here. If you save the part as external and use it in other assemblies, remember that it can change if the skeleton sketch changes. This can be good or bad depending on your intent but needs to be noted regardless.
    Like • Show 3 Likes3
    Actions
    - Tom Hickerson @ Jim Steinmeyer on Jul 11, 2017 11:29 AM
      Mark Correct
      Correct Answer
      Jim,
      
      I have tried what you mentioned. Create an assembly, insert my skeleton sketch, and then in the assembly inserting a new part. That all works, but then I have an assembly with two parts. When I try and edit the new part I just inserted it opens to a blank part. How do I go about being able to sketch on top of my skeleton sketch, or add weldment features?.
      Like • Show 1 Like1
      Actions
      - Jim Steinmeyer @ Tom Hickerson on Jul 11, 2017 12:07 PM
        Mark Correct
        Correct Answer
        Tom Hickerson,
        You are correct that you get a blank part to start. Actually when the part is inserted it will place the part on a surface that you pick and open the first sketch for you to start sketching. If that isn't what you want you can close the sketch and exit out of the new part. Click on the icon in the upper right corner to exit. This icon shows that you are editing a part or assembly within the top assembly.
        If the "edit Assembly " feature isn't open you can select a new part within the feature tree and RMB to get the option to edit it.
        
        When you have a part active it will show blue ( or a different color if you have changed it in System Options) in the feature tree so that you know that it is active. Now you can go about making drawings just as normal except you have the skeleton sketch and maybe any other parts that are in the assembly ahead of the new one to use for reference. When in a sketch you can use the convert entities feature to use existing sketches as usual. Matt Peneguy and Dan Pihlaja have some very good suggestions on what to look for. Isolating parts and sketches as John Stoltzfus teaches in Dan's note can be very helpful to ensure that you don't reference incorrect items in the assembly.
        (Didn't know you were going to have so much reading to do when you asked this question, did you?)
        Like • Show 1 Like1
        Actions
        Matt Peneguy @ Jim Steinmeyer on Jul 11, 2017 12:42 PM
        Mark Correct
        Correct Answer
        Tom Hickerson,
        Jim Steinmeyer makes some good points and there is a "learning curve" to this method. Most of it is training your brain to think the new way. It takes a while, but the pay off is that you end up with a robust assembly that you can modify anytime. Just keep in mind that if you create too many sketch relations, the sketch can "blow-up" on you just like lots of mates. So don't try to throw everything into a "master sketch", break up your sketches. Also only add the the driving information to the sketches. Though there is an urge to add all the geometry to the master sketch, don't. Keep those master sketches as bare bone as you can. For instance the line below represents the outside dimension for my tower machinery deck. I'll have a plane matched to that line in my structural, mechanical and electrical assemblies. Since my tower platform is symmetric, all I needed was that line showing the limits of the platform.
        Also, only drive 1 level deep with your sketches. If you have:
        ASSP>BSSP>CSSP
        CSSP can reference BSSP, but not ASSP. If you want to reference something from ASSP, it needs to be in BSSP, and then you can drive it to CSSP.
        Like • Show 0 Likes0
        Actions
  - Dan Pihlaja @ Tom Hickerson on Jul 11, 2017 8:46 AM
    Mark Correct
    Correct Answer
    Jim Steinmeyer is correct. Although you can do it your way as well....but in general, in context modeling (the way I take it) is using an assembly as the link between the two parts. Add both parts to the same assembly, then RMB on one of the parts and select "Edit Part". Then go forward with editing it.
    
    If you want them linked then make sure that the "No External References" button is turned off.
    Like • Show 2 Likes2
    Actions
Jim Steinmeyer Jul 10, 2017 4:51 PM
Mark Correct
Correct Answer
I haven't done this so i might be wrong but, It looks like the Blue Skeleton has a drop-down arrow beside it. If you expand it will that give you access to the skeleton sketch so you can hide it?
Like • Show 3 Likes3
Actions
- Craig Schultz @ Jim Steinmeyer on Jul 10, 2017 4:53 PM
  Mark Correct
  Correct Answer
  ^^^ Yep
  
  It should have all the folders that you imported (sketches, bodies, .....) underneath the imported part. You can select and hide from there
  Like • Show 2 Likes2
  Actions
- Tom Hickerson @ Jim Steinmeyer on Jul 10, 2017 5:20 PM
  Mark Correct
  Correct Answer
  Jim,
  
  That was what I needed to do. I guess I was used to hiding parts that way and forgot that it was a sketch in the part.
  Like • Show 2 Likes2
  Actions
John Stoltzfus Jul 11, 2017 6:14 AM
Mark Correct
Correct Answer
What you're showing here is that the Sketch is shown, click on the eye and it should hide it

If the eye is like this

Then you need to click it to Show

There are different ways to achieve your design intent as was pointed out by the others, the important part of using a Skeleton Sketch is the ability to have robust and parametric models. Just makes sure you're pushing information downhill and not pulling any information from another part or sketch that is lower in the feature tree. I prefer to have the Skeleton Sketch as a part and the first part in the assembly, that way I know that the information is going the right direction...
Like • Show 3 Likes3
Actions
Deepak Gupta Jul 11, 2017 6:18 AM
Mark Correct
Correct Answer
Expand it out and then go to sketch folder and you can hide sketch from there
Like • Show 3 Likes3
Actions
Matt Peneguy Jul 11, 2017 11:41 AM
Mark Correct
Correct Answer
Hey Tom Hickerson,
It looks like you are getting a lot of good advice here. I am new to this SSP method too, and have created a quick walk through that demonstrates some of the techniques I learned from John Stoltzfus and here on the forums. John has a lot of great tricks, such as using "Isolate" to make sure you aren't inadvertently working at the assembly level or on a part or sketch you don't intend to. I suggest you download the PDF at Skeleton Sketch Part Method for Large Assemblies and go through my simple example. That way you can hit the ground running without having to learn each individual tip.
And please let us know in this thread or over at the thread above if you learn any SSP tips and tricks that I missed.
Like • Show 3 Likes3
Actions
- Dan Pihlaja @ Matt Peneguy on Jul 11, 2017 11:43 AM
  Mark Correct
  Correct Answer
  Matt Peneguy wrote:
  
  Hey Tom Hickerson,
  It looks like you are getting a lot of good advice here. I am new to this SSP method too, and have created a quick walk through that demonstrates some of the techniques I learned from John Stoltzfus and here on the forums. John has a lot of great tricks, such as using "Isolate" to make sure you aren't inadvertently working at the assembly level or on a part or sketch you don't intend to. I suggest you download the PDF at Skeleton Sketch Part Method for Large Assemblies and go through my simple example. That way you can hit the ground running without having to learn each individual tip.
  And please let us know in this thread or over at the thread above if you learn any SSP tips and tricks that I missed.
  
  I am actually referencing his walkthrough. It is very thorough. Thank you for sharing it by the way.
  Like • Show 3 Likes3
  Actions

How to hide base sketch in skeleton sketch method?

Outcomes

Related Content

Recommended Content