This one has me a bit concerned. I'm not seeing how it is possible to extrude a surface at an angle base off an edge.
When I try to do this as an extrude operation I see that there is only the option to extrude from a sketch.
Many times it is necessary to extrude non-planar surfaces either based off of an edge or a curve.
Perhaps this can be done through a surfacing tool but I haven't found it yet.
I'm certain that this has to be possible. I'm hoping someone with experience can lend a hand.
Solved! Go to Solution.
A picture would help. However, from what I understood. The following video would help.
Thank you for your demonstration. Unfortunately this isn't the type of application I'm looking for.
I will attach an example of the issue I'm trying to resolve.
In the attached you will see 3 different labels.
SKETCH: I wish to develope a parting line with this sketch but there is a negative draft in the twisted parting line of the customer model (in the area where the sketch intersects into the model).
PARTING LINE: In the area with the label this would be negative draft if viewed from the bottom view. This needs to be pulled out a specific distance.
EDGE: This is the edge in which I'd like to extrude draft out to intersect with the depth of the parting line. I would transfer this new location into my sketch to obtain a parting line split that will be drafted both ways in the Z direction. The resulting drafted extrude will not remove material in the area of the EDGE. The draft will not be negative in either direction of the split.
The obvious way to move out my parting line sketch in the area shown would be by developing a drafted extrude off the specified EDGE area which would be intersected out on a parting line surface and be referenced into the sketch.
Is there any way I can get the needed drafted extrude?
Do you have the advanced surface extention?
Regardless, I would considere a Blend making sections in both (multiple) planes required to account for the draft. The sweep sections could be driven from a "draft" sketch in a plane normal to the sweep sections. For a more complex solution, a Swept-Blend might be more appropriate.
Can the feature be created easier without draft and drafted in a separate step?
I am not seeing exactly what you are doing.
I'll attach an example of the same area using our other CAD system.
The surface was done quite simply by extruding off the edge 5 degrees from the Z direction.
I have placed a curve that would intersect with the parting line on this extruded surface.
I would then use this curve on the updated sketch profile.
You can see part of the old "undercut" profile curve.
I'm looking for the best way to do this same thing in Creo.
I wouldn't be opposed to making the drafted extrude in seperate operations but the main struggle is getting an extrude from an edge.
We do have the ISDX surface package. Would this help in this application?
Sorry I am unclear with my earlier example.
I take it neither edge is planar? Projecting curves comes to mind. If I was looking at what I think you're looking at, I would go back to basics by remodeling the basic part minus draft and then apply drafts to a model with normal planes, and then re-applying the fillets. I take it you are trying to modify an existing part? Imported perhaps?
That is correct, the edge is not planar in this application. Very typically in our modeling we run into the need to borrow non-planar edges or curves.
We really don't have the option of removing draft to the customer model. The most significant reason is because the customer applied twist to the locked area of the parting line, that also twisted the draft. (This is what created the negative draft condition that we need to correct).
I am creating this part from scratch. The drafted surface I am after is only to obtain construction geometry for my part profile sketch.
I am searching for the same versatility that another person is looking for in the Product Idea area. "Use Boundary Edge to create Extrude or Revolve Feature" http://communities.ptc.com/ideas/1566
I am still holding out that someone will be able to present a viable way of getting what I am looking for without flat out guessing.
Sorry I couldn't help much. I have been in your position more than once. And I have to work with the basic package. In SW it would be simple.
In this case, I'd have to say the "Flexible Modeling Extension" could go a long way to simply cleaning up a single draft feature. Not sure how it would do on complex 3D curved faces, though.
Is it possible for the customer to provide the model without the edge radii? In Creo - Pro/E, things often go much easier without these radii. In that case, it would be much easier to cut out a section and replace it with some surface work and solidifying it. This is where matching the edge radii is most challenging.
I know I am just rambling here, but have you tried removing a section of the part and doing a sweep-blend for the section that needs to be corrected? I found a wonderful command in Brian's excellent tutorial on a tube weldment for creating a 3D spline from 2 planer sections using "intersect". This could create some very comprehensive guide curves.
I appreciate everyone's help in this thread. There are some useful ideas for other applications. After a lot of thinking I did discover a solution even though it did require extra steps. There certainly is a price to pay in learning the software. We are banking that with Creo's top rate tangency controls and parametrics that we will eventually end out much ahead.
My need was to extrude with a draft on a specified locked edge. This is what I needed to do to accomplish this:
1) Build sketch using profile of the needed edge.
2) Extrude this sketch in the Z direction
3) Draft this extrusion using the imported models edge as the hinge.
I still am crossing my fingers that eventually Creo will be able to extrude directly from an edge.
why don´t you create a plan with the angle you need, then you create another plan 90º from the first.
if you creat a sketch from the second plan, (using the project tool,and select the edge), when you extrude it will be with the correct angle...
you can also create a skirt surface (only on .MFG) and give the direction you want
You could also creat a flat surface, than you could add a draf split the draft from the
Hope it helps...
I tried your example out and it does allow a non-planar edge extrude at an angle without an extra step (as per my example).
I am very new with the software but the variable section sweep with this application appears the way I will want to make my varying draft angles as well.
I appreciate all the feedback!
Hopefully this thread will help other new users of Creo.
I still would love to simply extrude from an edge.
Nice thought, Antonio!
I ran into a need for this the other day and let a sweep resolve it.
The task naturally asks for an extrude and it is easy to focus on finding a solution in that direction.
I stumbled onto sweep expecting something totally different. This thread didn't even pop into my mind.
Gotta love this forum!