Trouble editing a sketch

[CGPM]

I have imported a DXF wireframe legacy model from my old cad program.  All of the layers are now separate sketches that I can edit, but no parametric modeling.  I enable "capture design history", right mouse click the sketch and I no longer have the option to edit the sketch.  The component the sketch is in is active.  What am I doing wrong?

[CGPM]

Oh come on, this shouldn't be that hard of a question to answer.  I have tried several new "uploads" of different wireframe models in both dxf and dwg with the same results.  I have the option of editing the sketch until I enable "capture design history", after which I no longer have the option to "edit sketch".  Is this to be expected or nuances of my old cad software?  I have 15 years of legacy cad in this old program, kind of important to get it to work.

[innovatenate]

The only thing I can think is that the sketches are coming in as part of a Base Feature. Perhaps you need to edit the Base Feature prior to editing the sketches? 

Are you right clicking on the sketch in the browser or in the Timeline to edit it?

Could you share an example file or a screenshot here? 

Thanks,

[CGPM]

You are right on all accounts with your first two sentences, thank you!  After enabling "capture design history" I right mouse cliked the base feature in the timeline that was just created and selected "Edit".  Now I have the option to edit my sketches.  When I click "Finish Base Feature" I can no longer edit my sketches.  There are no sketches in the timeline, just the one base feature created by enabling "capture design history".  Any pointers other than click "edit" on the base feature before continuing?  I will be creating a component for each sketch then moving that sketch to the component to continue modeling.

Here is one of the files I have imported.  Once imported there is one component and ten sketches representing the 10 layers I exported from my old cad program.  If you open this file you will understand why I am so thrilled to be moving to Fusion for my cad/cam needs.

Thanks again-

David

[CGPM]

Ps-  I don't find any information about "Base Feature" or "Edit Base Feature" in the learning resources section.  Where/ how should I look to learn more about this?

[innovatenate]

Just curious what application the DXF is coming from. Perhaps you could export a SAT or an IGES file and spare yourself the need to rebuild all of the solids... 

I'm not sure if I have any other tips to offer. Before you enable the timeline, you can right click on the ALUMINIUM DOOR ARM in the browser and select Create New Components (not while editing Base Feature). From there, you should be able to drag and drop sketches into the new components in the browser. If you do this before turning on the timeline, you can move the sketches into components. I believe this will create separate Base Features for each sketch. 

When you are editing a Base Feature you are in a Direct Model - edit mode in Fusion 360. While editing a Base Feature, commands are not captured in the timeline. 

I think this is one of the better features that explain Direct Modeling versus capturing design history and how you may be able to use the Base Feature command. 

http://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/video/youtube/watch-v-YJU4avXux2...

Let me know if that helps or if you have other questions.

Cheers,

[CGPM]

The cad/cam program this is comming from is Excalibur, which went out of business around 2001.  It was a surface modeler but if you are doing 2.5d machining you needed lines and arcs to program from, not surfaces.  All of my cad "models" are wireframe, and very limited to reduce the clutter when cam programming.  Dxf or dwg are the best formats to transfer my models to Fusion that I have available.

Thank you for mentioning that editing a base feature is in Direct Modeling mode, since I do want to do all fo my modeling in the parametric mode.  To do all work in the parametric mode would it just be best to create a sketch, project the imported sketch to it, then delete the imported sketch, for each sketch/ layer that is imported?  Or is there a better way?  If I am not being clear about what I need please let me know and I will do a better job of explaining it when I have more time.

Thank you for the video link, I did watch it.

[innovatenate]

By default, when you import data into Fusion 360 the timeline is disabled. If you enable timeline, the existing sketches, surfaces, or bodies are going to be available in Direct Modeling mode. You might think of this in a similar way to how Inventor would import a STEP file as a "Dumb Solid" (with no native features). 

If you are looking to utilize parameters to update the model (from within the parameters dialog), you will need to create the features outside of these Base Feature. The below youtube video shows how you can create features and dimensions that can be update parametrically.

http://www.youtube.com/watch?v=apkUQKNwHIo

For your sketches that are being imported in, is the goal to be able to modify these sketches in a similar fashion to the youtube video where you edit the value of a parameter? 

If yes, then you will need to create these sketches with dimensions while not in a base feature. You can copy and paste sketch entities. If you copy and paste, please note that you have to copy while editing the imported sketches and paste during the creation of a new sketch (with capture history enabled). One useful hint may be to use the "Move to Sketch Plane" command from the right click menu while selecting sketch entities.

You could also project the sketch entities as you mentioned. If you use the project, you can right click on the sketch entities and choose break link to begin to add dimension to the figures. 

If you don't really need the parameters, and are just looking to take advantage of the timeline for updating the model, you may consider building features outside of the base feature with the existing imported sketches. Downstream commands will update as the timeline computes each feature.

I hope that helps. Let me know if anything is unclear or if you have any questions.

Kind Regards,

[CGPM]

I don't need to be able to control the model/ sketches with parameters but do want to control the model with the sketch from which it is constructed.  This part is a replacement for one that failed on my cnc mill that I have reverse engineered.  Since the dimensions I have taken from the machine are not perfect I will be makeing small adjustments to get it to work right.  I would like to be able to make these adjustments to the sketch which in turn will modify the body.

Some of my "sketches" are 3D, not just 2D, since they originated from 3D wireframe models.

A new problem is I need to change the units from mm to inch and then scale everything up 2.54, but when I try I can't select any geometry to scale.

Is any of the information I need in the Learning resources?

Thank you for your help-

David

[innovatenate]

Have you tried using the scale tool from the Model > Modify drop down menu?

There is a short video in the learning section on scaling.

http://help.autodesk.com/cloudhelp/ENU/Fusion-Form/files/GUID-D3F6F79B-1498-48B3-B98C-7D57B620005A.h...

It doesn't show the scale tool working on a sketch, but it will work in a similar fashion. Does this answer your question? 

I've made a quick screencast that shows how you might get started.

Let me know if it helps.

Thanks,

[CGPM · Accepted solution]

Thank you for the video, it answered around a dozen questions I have.  Great to see someone who really knows how to use the program do to my model what I need to do, especially since I have so many models like this to bring into Fusion.  I was trying to scale correctly, I just was trying to select the geometry with a selection window or left mouse clicking with my cursor, neither of which would work.  When I selected it with the browser it worked fine.

Thanks again for all of your help-

David