Modifying andymark drivetrain cad

We build andymark standard tank drivetrain but we chose to use square config but a bit narrower like the long chassis. Our cad team struggle to modify it. They cant delete or modify things.

Does someone know how to solve it
/ have editable cad of theese
/ have cad of config we want.

We want the sides c panel the way that the screws are accesible from outside
Am14u4 manual i believe

If you downloaded the assembly STEP from AndyMark then you should be able to save it as an assembly in your CAD software’s format; that should also extract the individual parts. Usually, you need to manually add new assembly constraints.

Your CAD software should allow you to add features to the existing STEP files for each part. For example, if you need to shorten a piece or add holes, you would put in extrusions that remove material.

so we just have to convert STEP to editable for SOLIDWORKS and it will be easily editable? (shortening, deleting parts)

The parts from the step file will be solid bodies at that point, so it wont be as simple as changing an extrude feature’s length. But yes, thats effectively it.

I would just find the part you need to edit, create a new sketch, add a box around the section you no longer want, then extrude-cut it away.

Should be. Fletch described it well. I’ve forgotten exactly what Solidworks does, but the first feature in your model tree will be something like an “import body” that is the un-editable STEP file, and you will then add your new features onto it. The assembly will behave like a normal Solidworks assembly but the parts will usually be unconstrained, so you have to add that yourself to move the parts into the right places.

There may be one additional thing you may need to do when importing the part – independent of what has been posted so far.

There’s a SW feature called “3D Interconnect” (SOLIDWORKS 3D Interconnect - 2020 - SOLIDWORKS Help) – the short of it is, if it’s enabled, you can bring in parts not created in SW, but they won’t be editable. You can identify when enabled on parts/assemblies by the green arrows on the icons in the feature tree. See the figure labeled “3D Interconnect Reference Tree”: 3D Interconnect makes SOLIDWORKS 2017 a true Multi-CAD environment

To turn that off globally (as opposed to breaking the links within one file), it’ll be within the Open dialog; click on the file you want to open, but before you click the Open button, click “Options…”:

Choose “Import” in the left pane
Choose “General” in the top drop-down
Uncheck “Enable 3D Interconnect”.
Click OK in the System Options dialog
Finally, click OK in the Open dialog

STEP files in general do not have the necessary parametric data to make parts editable. This is just due to the nature of it’s purpose as a universal file that can be opened in various other software.

There is a feature called Featureworks in SOLIDWORKS that can reverse engineer a STEP file, creating an editable file from that. I’ve rarely found it successful or worth the effort. But I haven’t tried it with the kit bot chassis, so maybe worth a try.

Typically if you want to edit a STEP file, you make a sketch of the profile and recreate it manually, cut and remake whatever features you want. But FIRST I usually separate the bodies, save each as their own part, then create a new assembly. That makes the editing and manipulation easier, more controlled.

In this case, you really only can remove material to edit a part. So it should be straight forward to just cut what you want once you have each part separated.

I’m a little surprised a native, well-made kit bot file in SOLIDWORKS hasn’t already been available…

A big problem in the andymark step file is also the random and unhelpful generation of the center point and midplanes of the assembly. It unfortunate because it’s a hurdle beginner teams that use the file need to deal with.

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